Copyright: Copyright ® 1995 by MicroSim Corporation


 Schematics Help Contents
To learn how to use Help, press F1

Overview

Using the Symbol Editor

Configuring the System

Using the Schematic Editor

Command Summary

Drawing a Schematic

Drawing Wires and Busses

Placing Parts

Using Ports

Connecting to Power and Ground

Adding Text

Editing a Schematic

Selecting Items on a Page

Moving Parts, Wires and Text

Using the Cut, Copy and Paste Commands

Editing Attributes

Editing and Viewing Symbols

Panning and Zooming

Managing Schematics

Creating a New Schematic

Opening and Saving Schematics

Creating a Multi-page Schematic

Creating a Hierarchical Schematic

Configuring Symbol Libraries

Setting the Page Size


Overview

Schematics is a schematic capture front-end program.  It is designed to provide a convenient, easy-to-use system for creating and managing circuit drawings.  These drawings may be single-page, multi-page and/or hierarchical.

Schematics includes netlisters for popular PCB layout formats as well as tightly integrated interfaces with MicroSims other tools for simulation (MicroSim PSpice/PLogic), analog optimization (MicroSim PSpice Optimizer), PCB layout (MicroSim PCBoards), signal integrity analysis (MicroSim Polaris), and PLD synthesis (MicroSim PLSyn)

Schematics includes a fully integrated Symbol Editor for creating and changing symbols.  You can view, change or create symbols in the midst of editing your schematic.


Using the Symbol Editor

Command Summary

Managing Symbol Libraries

Invoking the Symbol Editor from the Schematic Editor

Editing Symbols

Creating New Symbols

Adding Pins

Adding Symbol Graphics

Editing Attributes in the Symbol Editor

Changing the Origin of a Symbol

Resizing the Bounding Box


Configuring the System

Setting the Display Colors

Configuring a Text Editor

Using the MSIM.INI Configuration File


Schematic Editor Function Keys
Schematics Keyboard Commands

Schematic Editor Function Keys

F1	On-Line Help

F2	Move to lower level in the schematic hierarchy

F3	Move up one level in the schematic hierarchy

F4	Text Stay on Grid On/Off

F5	Orthogonal On/Off

F6	Stay on Grid On/Off

F7	Auto-Increment On/Off

F8	Auto-Repeat On/Off

F9	Rubberband On/Off

F10	View Errors

F11	Run PSpice

F12	Run Probe

For those items which turn a feature on/off, press the  function key to turn the feature on.

Press the Shift key  the function key to turn the feature off.

Schematic Editor Shortcut Keys

Press the key combination to directly invoke the menu item.

Space Bar	Draw/Repeat

CTRL+A	View/Area

CTRL+B	DrawBus

CTRL+C	Edit/Copy

CTRL+D	Draw/Rewire

CTRL+E	Edit/Label

CTRL+F	Edit/Flip

CTRL+G	Draw/Get New Part

CTRL+I	View/In

CTRL+L	View/Redraw

CTRL+M	Markers/Mark Voltage Level

CTRL+N	View/Fit

CTRL+O	View/Out

CTRL+P	Draw/Place Part

CTRL+R	Edit/Rotate

CTRL+S	File/Save

CTRL+T	Draw/Text

CTRL+U	Edit/Undelete

CTRL+V	Edit/Paste

CTRL+W	Draw/Wire

CTRL+X	Edit/Cut


Symbol Editor Function Keys
Symbol Editor Keyboard Commands

Symbol Editor Function Keys

F1	On-line Help

F2	Grid On/Off

F4	Text Stay on Grid On/Off

F5	Auto-Scroll On/Off

F6	Stay on Grid On/Off

F8	Auto-Repeat On/Off

F10	Current Errors

For those items which turn a feature on/off, press the function key to turn the feature on.  Press the Shift key  the function key to turn the feature off.

Symbol Editor Shortcut Keys

Press the key combination to directly invoke menu Items.

Space Bar	Graphics/Repeat

CTRL+A	View/Area

CTRL+C	Edit/Copy

CTRL+D	Part/Definition

CTRL+E	Packaging/Edit

CTRL+F	Edit/Flip

CTRL+G	Part/Get

CTRL+H	Edit/Change

CTRL+I	View/In

CTRL+L	View/Redraw

CTRL+N	View/Fit

CTRL+O	View/Out

CTRL+P	Part/Pin List

CTRL+R	Edit/Rotate

CTRL+S	File/Save

CTRL+T	Edit/Pin Type

CTRL+U	Edit/Undelete

CTRL+V	Edit/Paste

CTRL+X	Edit/Cut


Schematic Editor Menu Summary

File Menu	Opens and saves files and prints schematics.

Edit Menu	Modifies or deletes items on the current schematic page.

Draw Menu	Draws wires, buses, and places parts on the schematic.

Navigate Menu	Allow user to select page or change level of hierarchy while editing.

View Menu	Changes the viewing scale on the schematic, redraw.

Options Menu	Sets up the display and hard copy environment.

Analysis Menu	Creates a netlist, sets up analyses, and runs simulations.

Tools Menu	Allows you to interface to external layout editors.  You can create netlists that can be used as input to your layout editor, and apply backward ECO's 	generated by the layout editor to the schematic.

Markers Menu	Place and manipulate markers that enable you to select points from the schematic that you wish to view from within Probe.

Window Menu	Create and close windows.

Help Menu	Provides context-sensitive help on all aspects of the schematic editor.


Schematic Editor File Menu
File Menu

Opens and save files, establishes a new workspace, and prints copies of the schematic.  For more information, see the File Menu items in the list below:

New	Starts a new schematic.

Open	Opens an existing schematic for editing.

Close	Closes the schematic in the active schematic window.  Any other windows showing that schematic are also closed.

Import	Imports a schematic created with OrCAD.

Save	Saves changes to the current schematic file.

Save As	Saves the currently active schematic to  a different file name.

Print	Prints one or more pages of the currently active schematic.

Printer Select	Changes the default printer used by Schematics.  Also allows setting up various printer options, such as landscape or portrait mode, paper size, and printing resolution.

Edit Library	Brings up the Symbol Editor so that you can edit a symbol in the library.

Symbolize	Creates a symbol to represent the current schematic, creating pins for each interface port

Reports	Creates a Bill of Materials report.

Current Errors	Displays the list of current errors.  For errors which occur while performing the ERC or  creating the netlist, errors contain the location of the error.

Exit	Exits Schematics.


Schematic Editor Edit Menu
Edit Menu

Edits the graphics and part definition of the current part.  For more information, see the Edit Menu items in the list below:

Undelete	Restores the last item(s) deleted with the Delete or Cut command.

Cut	Deletes the currently selected item(s)  and saves it to the paste buffer

Copy	Copies the currently selected item(s) to the paste buffer

Paste	Places the items in the paste buffer onto the page.

Copy to Clipboard	Copies a selected rectangle on the schematic to the Windows clipboard.

Delete	Deletes the currently selected items.

Attributes	Edits the attributes of a selected item(s).

Label	Places a label on selected wires, bus segments, or ports.  Wire and bus segments  may display multiple labels; however, all labels for a segment will contain the same text.

Model	Allows editing of  the simulation .MODEL or .SUBCKT representation of a part.  From the schematic editor the user can rename the model or subcircuit used or edit a copy of the underlying model or subcircuit.

Stimulus	Invokes the stimulus editor on the currently selected stimulus part.  If no stimulus is currently selected, allows you to modify all stimulus on the page or in the schematic.

Symbol	Invokes the symbol editor on the symbol for the currently selected part.

Views	For selected hierarchical blocks, allows assigning of subschematic(s) and view(s).  For hierarchical symbols, views are displayed but can only be changed from the Symbol Editor using the Edit/Set Schematic command.

Convert Block	Converts the selected block to a symbol.

Rotate	Rotates a selected object(s) 90 degrees counterclockwise.  The selected object(s) rotates around the center of the selection box.

Flip	Creates a mirror image of the selected object(s).

Align Horizontal	Moves all selected objects so that their origins are along the same horizontal line.

Align Vertical	Moves all selected objects so that their origins are along the same vertical line.

Replace	Replaces all currently selected parts with a new part type.

Find	Searches current schematic page for components that match attribute values specified by user.


Schematic Editor Draw Menu
Draw Menu

Draws wires, buses, and places parts on the schematic.  For more information, see the Draw Menu items in the list below:

Repeat	Repeats the previous menu command.

Place Part	Places an instance of the current part (as previously specified in the Get New Part Command) onto the schematic.

Text	Places text on the schematic.

Wire	Draws a wire.

Bus	Draws a bus.

Block	Creates an empty block that may then be moved and sized by the user.

Get New Part	Allows you to enter the name of a part to be placed on the schematic, or to browse the libraries to choose a part.

Rewire	Reroutes a wire or bus segment without changing its endpoints.


Schematic Editor Navigate Menu
Navigate Menu

Allows you to move from page to page and through the hierarchy.  Also allows you to create or delete pages.

Previous Page	Loads the previous page for editing.

Next Page	Loads the next page for editing.

Select Page	Loads a particular page of the schematic for editing.

Create Page	Adds a new page to the current schematic.

Delete Page	Deletes the current schematic page.  You must confirm the deletion.

Copy Page	Copies a page(s) from a schematic into the current schematic.  In the dialog box, specify the name of the schematic you want to copy from, the directory in which it is found, and the page number(s) to copy.

Edit Page Info	Edits the title of the schematic page.  The page title can be used in the title block.

Edit Schematic Instance
Opens an existing schematic file for editing.

Edit Schematic Definition
Opens an existing schematic file for editing.

Push	Push down a level in the currently selected component.

Pop	Pop up a level from the current schematic.  If the user had pushed into a schematic page from the symbol editor they will be returned to the symbol editor.  If the user had pushed into a hierarchical component they will be returned to the page of that component in the schematic editor.

Top	Pop back up to the topmost level of the current schematic or symbol.

Where	Displays the complete hierarchical path of the current schematic page being edited.


Schematic Editor View Menu
View Menu

Changes the viewing scale on your schematic.  For more information, see the View Menu items in the list below:

Fit	Sets the viewing scale to show all parts, wires and text within the viewing window.

In	Allows you to view an area on the schematic at closer range (i.e., to magnify the area).

Out	Changes the viewing scale so that you can view the schematic as if from a greater distance away (i.e., to view more of the schematic on the page at one time).

Area	Allows you to select a rectangular area on your schematic to be expanded to fill the screen.

Previous	Restores the previous area that was displayed.

Entire Page	Allows you to view the entire schematic page at once.

See Also

Using the View Menus

Redraw	Redraws the screen display.

Pan-New Center	Retains the current zoom factor and pans the schematic so that the point selected is centered in the display.


Schematic Editor Options Menu
Options Menu

Sets up the display and hard copy environment and turns on automatic features.  For more information, see the Option Menu items in the list below:

Display Options	Allows you to set up your display from a list of options appearing in the dialog box.  Choose from the following options:

Grid On

Snap to Grid

Orthogonal

Stay on Grid

Rubberband

Status Line

Cursor X and Y

Grid Spacing

Text Grid

Page Size	Sets the page size (i.e., the drawing size such as A-size or B-size) in inches or millimeters.

Auto-Repeat	Automatically places an object(s) identical to the previously placed object a specified distance apart.  Use the Repeat function from the Draw Menu to continue the action.  You can use Auto-Repeat with the Place Part command to place repeated part instances, or with the Wire command to place wire segments.

The Horizontal and Vertical Offset fields automatically place a new object(s) a specified distance from the previous instance.

Auto-Naming	Automatically assigns a reference designator whenever you place a part.  In the dialog box, you can turn Enable Auto-Naming and Enable Auto-Increment on or off.

The Starting Designator No. sets a number from which the automatic reference designator will begin numbering, if Enable Auto-Increment is turned on (enabled).

Label Template allows you to specify a label for wires, buses, or ports on your schematic.  The number will automatically increment if Auto-Increment is turned on.

Set Display Level	Turns display of text on/off for the screen, on the hard copy, or on both.

Editor Configuration	Allows you to define parts libraries, library paths, autosave intervals, default page settings and application settings.

See Also

Setting the Display Colors

Defining the Default Settings

Pan & Zoom	Sets the parameters for panning and zooming..

Restricted Operations	Enables and disables whether separate wires with the same label are merged into the same net or whether offpage ports are required.

Translators	Allows you to associate views with schematic translators.  An example of this is the view called PSVIEW that is used by the Simulation netlister.


Schematic Editor Analysis Menu
Analysis Menu

Creates a netlist, sets up analyses, and runs simulations.  For more information, see the Analysis Menu items in the list below:

Electrical Rule Check	Performs an electrical check of the schematic.  This command checks the connections on the schematic against a set of electrical standards.  To view any errors, choose File/Current Errors.

See Also

Performing an Electrical Rule Check

Create Netlist	Generates a simulation netlist for the current schematic.  A netlist shows all of the components, their interconnections, and their values.

See Also

Creating a PSpice/PLogic Netlist

Setup	Specifies which types of simulation analyses are enabled, and allows user to set up the parameters for selected analyses.

Library and Include Files

Allows you to specify a list of files that will be included in the simulation netlist.  Model library files are added with the .LIB command, stimulus library files with the .STMLIB command, and include files are added with the .INC command.

Simulate	Performs a circuit analysis on the current schematic.  Choosing this command automatically executes the following (if necessary):  annotation, electrical rule check (ERC), and netlist.

See Also

Running a Simulation

Using Special Symbols to Invoke Simulation Cmds

Specifying Output Variables

Probe Setup	Allows setting of whether Probe will automatically be started during/after a simulation and whether data for all nodes should be saved.

Run Probe	Allows you to view the simulation results in graphical form.  A successfully completed simulation produces a .dat file for use with Probe.

See Also

Specifying Output Variables

Examine Netlist	Allows you to examine the netlist file.

Examine Output	Allows you to examine the output file (.out), which is created by running a simulation.


Schematic Editor Tools Menu
Tools Menu

The Tools menu allows you to interface to external layout editors.  You can create netlists that can be used as input to your layout editor, and apply backward ECO's generated by the layout editor to the schematic.

Annotate	Assigns a unique reference designator for parts in the current schematic.  All parts must have a reference designator assigned before generating a netlist.

See Also

Annotating Your Schematic

Create Layout Netlist	Generates a layout netlist in the currently configured layout editor format.  A layout netlist consists of part and connectivity information needed by the layout editor.

Run Layout Editor	Starts the currently configured layout editor.

Back Annotate	Allows you to back annotate a schematic using an ECO file generated by a layout editor.

Configure Layout Editor

Allows you to select the layout editor format to be used.  Netlist File Extension specified the default file extension for the selected layout editor.  ECO specified the default file extension for ECO files for the selected layout editor.  Command Line allows you to specify the command to invoke the selected layout editor.

Browse Netlist	Allows you to examine the current layout netlist.  Schematics automatically brings up the configured text editor which displays the layout netlist.  You can select a different text editor by editing "msim.ini".

View Package Definition

Displays the package definition for the currently selected part.

Create Subcircuit	Creates a subcircuit netlist for the current level of hierarchy and all lower levels.  This netlist will be written to "<schematic name>.sub" (not the usual ".net" file).  At the current level of hierarchy, interface ports will be mapped into subcircuit interface nodes.  Note that if you made changes to the current level, you should save the changes before invoking the Create Subcircuit command.


Schematic Editor Markers Menu
Markers Menu

The Markers menu allows you to place and manipulate special objects called markers.  After a schematic is simulated and the Probe waveform analyzer is invoked, markers enable you to visually indicate points on the schematic where you wish to see voltages and current waveforms shown in Probe.

Placing a marker allows you to position one or more markers on the current page of the schematic.  If Probe is running and the schematic is not stale, Probe will be updated to show the specified waveform.

Mark Voltage/Level	Marks the voltage or digital signal at a net.  Net markers must be placed on labeled wires or on a pin.

Mark Voltage Differential

Marks the voltage difference between two nets.  Differential markers consist of a pair of objects, one for the "" node and one for the "-" node.  Each object must be placed on a labeled wire or at a pin.

Mark Current Into Pin	Marks the current into a terminal of a three-terminal or four-terminal PSpice device, (e.g., Bipolar transistor, MOSFET, JFET, or GaAs MESFET), or the current through a two terminal PSpice device, (e.g., resistor, capacitor, diode).  If placed on any other type of device, a warning will be given and the marker will be ignored.

Mark Advanced	Displays a list of the available markers.  This allows you to place markers to view magnitude in decibels, phase and/or group delay.

Clear All	Deletes all markers on all pages of the schematic.

Show All	Updates Probe with waveforms for all markers on all pages.

Show Selected	Updates Probe with waveforms for all currently selected markers.


Schematic Editor Window Menu
Window Menu

The Window Menu provides context-sensitive help on all aspects of the schematic editor.  For more information see the  Help Menu items in the list below:

New	Creates a new window showing the same schematic page as the currently active window.

Close	Closes the currently active window.

Arrange	Arranges the windows (either tiled or cascaded).


Schematic Editor Help Menu
Help Menu

The Help Menu provides context-sensitive help on all aspects of the schematic editor.  For more information see the  Help Menu items in the list below:

Contents	Lists the main topics available in the Help Menu.

Keyboard	Lists the function keys and shortcut commands.

Menu Commands	Provides help on all menu commands.

Using Help	Provides a tutorial on how to use this help system.

About	Displays the program version and customer ID#.


Symbol Editor Menu Summary

The symbol editor commands allow you to create and edit symbols for use in the schematic editor and to edit the parts in the component libraries.

File Menu	Creates and edits libraries and prints copies of part definitions.

Edit Menu	Edits the graphics and part definition for the current part.

Graphics Menu	Adds graphics and pins to the current part.

Part Menu	Creates new parts and edits parts from the current library.

Packaging Menu	Creates and edits package definitions.

View Menu	Changes the viewing scale on the current part.

Options Menu	Sets up the screen display and turns on repeating functions.

Window Menu	Sets up the screen display and turns on repeating functions.

Help Menu	Provides context-sensitive help on all aspects of the symbol editor.


Symbol Editor File Menu

Creates and edits libraries and prints copies of part definitions.  For more information, see the File Menu items in the list below:

New	Creates a new library file.  A bounding box appears in which you can create a symbol, and the title bar indicates that the file is "<new>."  You will be prompted for a name if you attempt to save the file.

Open	Opens an existing library file for editing.

Close	Closes the symbol editor, returning you to the schematic editor.

Save	Saves the changes to the current symbol.

Save As	Saves the current library and any changes to the current symbol to a new file name.

Print	Prints a hard copy of selected symbols from the current library.

Printer Select	Sets the default printer used by Schematics.  Also, allows you to set up various printer options, such as landscape or portrait mode, paper size, and printing resolution.

Current Errors	Displays the list of current errors.

Exit	Exits Schematics.


Symbol Editor Edit Menu

Edits the graphics and the definition of the current part.  For more information, see the Edit Menu items in the list below:

Undelete	Restores the last item(s) deleted.

Cut	Deletes selected objects from a symbol.  The deleted item(s) remain in a buffer for use with the Paste command.

Copy	Copies an item(s) for pasting.

Paste	Places the last item(s) stored with the Cut or Copy commands onto the symbol.  Click left to place the item(s) at the current cursor location.

Delete	Copies an item(s) for pasting.

Change	Allows you to edit selected pins, text, or attributes associated with a symbol.

Pin Type	Acts as a toggle to set the default pin display type for selected pins.

Model	Edit the simulation .MODEL or .SUBCKT representation of a part.  From the Symbol Editor the user can create/edit the model or subcircuit definition for the part.  This definition will be used by the simulator for circuit simulation.

Stimulus	Invokes the Stimulus Editor on the stimulus definition for a stimulus symbol.

Push	Pushes into the schematic represented by a hierarchical symbol.

Set Schematic	Allows you to assign schematic(s) and view(s) to the symbol being edited.

Check Schematic	Checks if the interface, global ports, and global nets of the schematic(s) assigned to this symbol match the pins and hidden pins of the symbol.  The user may change the symbol to correct errors, but the schematic must be edited in the schematic editor.

Rotate	Rotates a selected object(s) 90 degrees counterclockwise.  If you select an area of your schematic, the area is rotated around the center of the selection box.

Flip	Flips a selected object(s) to produce a mirror-image of the object.

Align Horizontal	Moves all selected objects so that their origins are along the same horizontal line.

Align Vertical	Moves all selected objects so that their origins are along the same vertical line.


Symbol Editor Graphics Menu

Adds graphics and pins to the currently selected part.  For more information, see the Graphics Menu items in the list below:

Arc	Draws an arc.

Box	Draws a box.

Circle	Draws a circle.

Line	Draws a line.

Pin	Adds a pin to a symbol and allows you to edit its name and number, if desired.

See Also

Creating Symbol Graphics

Text	Adds a text string.

See Also

Adding Text

BBox	Resizes the bounding box that surrounds a symbol.

See Also

Resizing a Bounding Box

Origin	Allows you to edit the origin, or reference point, for a part.

See Also

Changing the Origin of a Symbol

Repeat	Repeat the last command.


Symbol Editor Part Menu

Creates new parts and edits parts from the current library.  For more information, see the Part Menu items in the list below:

New	Allows you to create a new part for the library.

Copy	Copies an existing part from one of the libraries and makes it the current part.

Get	Allows you to select a part to edit from the current library.  This part becomes the current part, and is displayed in the main symbol editor window.

Remove	Delete one or more part(s) from the current library.

Save To Library	Saves the symbol to a different library.

Attributes	Allows you to define new part attributes or to modify existing attributes.  You can also change any system attribute (a system attribute is a required attribute).

See Also

Editing Attributes in the Symbol Editor

Definition	Changes the  part definition.  This command allows you to modify the description, part name, alias list, AKO name, and type.

Pin List	Allows you to edit all of the pins in a part using one dialog box.

See Also

Editing Pins

Get Symbol Graphics	Imports the graphics from an existing symbol onto the current symbol.  Only the graphics portion of a symbol is imported.  In the dialog box, specify the part name for the symbol to be imported.  You may use this command with any type of symbol.

Export	Writes the part definitions chosen from the list of parts in the current library to a text file and gives them a .sym extension.  This command allows you to transfer symbols from one library to another, or from one platform to another.  It allows you to manipulate individual symbols as files.

Import	Reads the text file with a .sym extension and makes it the current part; it can then be saved to the current library.


Symbol Editor Packaging Menu

Maintains the package definitions in the Package Library corresponding to the current Symbol Library file.  With this menu you can edit package types, gate types, pin assignments, shared pins, and attributes associated with the package definitions used for packaging for layout.

New	Creates a new package definition.

Copy	Creates a new package definition from an existing definition.

Get	Allows editing of any package definition in the current Package Library file.

Remove	Deletes a package definition.

Edit	Edits the package definition for the current symbol.  If no package definition exists, one is created.

Configure Package Types

Allows editing of the list of known package types (footprints) and package classes.

Export	Writes one or more package definitions to an ASCII text file.

Import	Reads a package definition from an ASCII text file and adds it to the current Package Library file.


Symbol Editor View Menu

Changes the viewing scale on the current part.  For more information, see the View Menu items in the list below:

Fit	Resets the viewing scale so that all graphics and text are visible.

In	Allows you to view an area on the symbol at closer range (i.e., to magnify).

Out	Changes the viewing scale so that you can view the symbol at a greater distance away (i.e., to view more of the symbol on the page).

Area	Allows you to select a rectangular area on your symbol to be expanded to fill the screen.

Previous	Copies an item(s) for pasting.

Entire Symbol 	Allows you to view the area enclosed by the symbol's bounding box.

See Also

Using the View Menus

Redraw	Redraws the screen display.

Pan - New Center	Maintains the same viewing scale but changes the center to the window to the point selected.


Symbol Editor Options Menu

Sets up the display and turns on repeating functions.  For more information, see the Options Menu items in the list below:

Display Options	Allows you to set up your display from a list of options appearing in the dialog box.  Choose from the following options:

Grid On
Snap to Grid
Stay on Grid
Auto-Scroll
Status Line
Cursor X and Y
Grid Spacing
Gravity
Text Stay on Grid
Spacing

Auto-Repeat	Automatically places an object(s) identical to the previously placed object a specified distance apart.  Use the Repeat function to continue the action.  In the dialog box, you can turn Enable Auto-Repeat on or off;  Horizontal and Vertical Offset automatically places new objects a specified distance from the previous instance.

Set Display Level	Allows you to choose whether to have the text or certain other components displayed on the screen, on the hard copy, or on both.

Pan & Zoom	Copies an item(s) for pasting.


Symbol Editor Help Menu

The Help Menu provides context-sensitive help on all aspects of the symbol editor.  For more information see the Help Menu items in the list below:

Index	Lists the main topics available in the Help Menu.

Keyboard	Lists all of the function keys and shortcut commands.

Menu Commands	Provides help on all menu commands.

Using Help	Provides a tutorial on how to use this help system.

About	Displays the software version and customer ID#.


Setting the Display Colors

You can change the colors that Schematics uses for the background, drawing wires, buses, parts and a variety of other items.

To change colors:

1.	Use a text editor ( e.g., Notepad) to bring up the msim.ini file, which is located in the Windows directory.  This file contains the default settings for Schematics.

2.	In the [Schematics Colors] section of the msim.ini file, add or modify an entry using this format:

<item name>=<color>

For  example, "wire=red" results in all wires being drawn in red.

Valid item names are as follows:

Item Name	Description

attributes	part attributes

background	window background

border	border

bus	buses

foreground	default for items not explicitly specified

grid	grid dots

hiddenpins	hidden pins

junction	junctions

marker	marker symbols for marker interface

pageboundary	page bounding box

pin	symbol pins

pinname	pin name text

pinno	pin number text

plsyn	PLSyn parts

port	port symbols

portlabel	port labels

refdes	part reference designator

selection	selected objects

stimulus	Stimulus Editor symbols

symbols	symbol graphics

symnames	part names

symtext	symbol text

text1	text layer 1

text2	text layer 2

text3	text layer 3

text4	text layer 4

wire	wires

wirelabel	wire labels

Valid color names are as follows:

black

blue

green

cyan

red

magenta

yellow

brightwhite

brown

lightgray

darkgray

darkblue

darkgreen

darkcyan

darkred

darkmagenta

Alternatively, you may specify varying degrees of color by using the R, G, B value of the color, where the range is from 0-255.

For example, wire=255 0 0 is the same as wire=red.

See Also

Using the msim.ini Configuration File


Configuring the Text Editor

By default, Schematics uses NotePad to display text files such as netlists, simulation out files, etc..

To change the text editor used by Schematics:

1.	Use a text editor ( e.g., Notepad) to bring up the msim.ini file, which is located in the Windows directory.  This file contains the default settings for Schematics.

2.	In the [MicroSim] section of the msim.ini file, add or modify the EDITOR entry using this format:

EDITOR=<editor command> %f

where %f specifies where the file name will be substituted on the command line.

This will change the text editor used by all MicroSim programs.


Configuring Optional Items

The majority of configuration items are set via menu commands in Schematics.  However, there are some that can be changed only by using a text editor to modify the configuration file, msim.ini.

[MICROSIM] Section Items

BACKUP	Specifies the directory in which backup copies are to be placed.  This location is initially set in the installation program.  Use the following format:

BACKUP=<directory>

EDITOR	Specifies the text editor to use for browsing files.  Use the following format:

EDITOR=<editor command> %f

where %f specifies where the file name will be substituted on the command line.

PLSYNCMD	Command line to invoke the PLSyn program.

 	Command to invoke the PLogic simulator.

POLARISCMD	Command to invoke Polaris.

PROBECMD	Command to invoke Probe..

PSPICECMD	Command to invoke the PSpice simulator.

STMEDCMD	Command to invoke the Stimulus Editor.

[Schematics] Section Items

LARGERESISTOR	Specifies the value for large resistors that are hooked to unconnected analog pins by the PSpice netlister.  Use the following format:

LARGERESISTOR=<value>

<value> defaults to {1/GMIN}.

MAXERRORS	Specifies the maximum number of errors shown in the View Errors dialog.  The default is:

MAXERRORS=500

NLTEMPLATE	Specifies the format the simulation netlister uses for creating node names.  Use the following format:

NLTEMPLATE=<prefix>%[min. width]ld

where ld MUST be lower case.  The default is $N_%04ld

TEXTHEIGHT	Specifies the size of 100%-sized text in 1/100" units.  The default is 8.  Use the following format:

TEXTHEIGHT=n

VIEWFITPERCENT	Specifies how closely the contents of the window fits the window size when a View/Fit is done.  The value must be between 50 and 100 and represents the percentage of the total area occupied by the image.  The default is 95.

ZOOMDELTA	Specifies the percent change in the zoom factor when a View/In or View/Out is done.  The default is:

ZOOMDELTA=20

See Also

Using the msim.ini Configuration File


Setting Up the Display Options

Allows you to set up your display.

To set up the display options:

1 Choose Display Options from the Options Menu.

2 Choose which of the following options you wish to have enabled:

Schematic Editor

Auto-Scroll

Cursor X and Y

Grid On

Grid Spacing

Orthogonal

Rubberband

Snap to Grid

Stay on Grid

Status Line

Text Grid

Symbol Editor

The symbol editor provides the options listed above, plus it allows you to specify the Gravity.

3 Choose OK.


Setting the Page Size

Schematics supports page size A-E and metric page size A0-A4.  You may also set up your own custom page size.

To Change the Page Size of an Existing Page

1.	Choose Page Size from the Options Menu.  This will show you the current page size.

2.	Choose a page size from the dialog box, or choose User-Defined and define your own dimensions.

3.	Choose the OK button.

This will change the page size for the currently active page.  It will also change default so that all new pages created will be created with this page size.

Each page size (A-E, A0-A4) has associated with it:  paper size (fixed), drawing area and pin-to-pin spacing.  To change these, see the Page Settings dialog in Editor Configuration command.


Defining the Default Settings

You may change the default settings through the Editor Configuration item on the Options Menu or through the msim.ini file.

To change the default page settings:

1.	Choose Editor Configuration from the Options Menu.

2.	In the dialog box, select the page setting you wish to modify.

3.	Select the Page Settings button to bring up the Page Settings dialog box.

4.	To modify the drawing area, enter a new length and width to suit your needs.

5.	To modify the pin-to-pin spacing, increase the number value, which causes the symbols to appear larger when printed, relative to the drawing area; decrease the number value to cause the symbols to appear smaller when printed.

6.	If you wish to modify the border type, choose a different border type from the Border Symbol section of the Page Settings dialog box.

To change any other default settings:

1.	Choose Editor Configuration from the Options Menu to change any of the default settings except the color, or,

2.	Use the msim.ini Configuration File to change any of the default settings.

See Also

Using the msim.ini Configuration File

Modifying the Libraries

Setting the Library Path


Using the MSIM.INI Configuration File

The msim.ini file is a text file which contains Design Center configuration settings.  You can modify this file using any text editor.  Many of the default settings except the color setting may also be modified through the Editor Configuration menu item in the Options Menu.

To use the msim.ini file:

1.	Use your text editor to bring up the msim.ini file, which is contained in your Windows directory.

2.	Modify the settings to suit your needs.

See Also

Defining the Default Settings

Setting the Display Colors

Configuring Optional Items


Using the Mouse

The mouse allows you to select and deselect items on your schematic, in order to perform an action.

Button	Action	Function

Left	Single click	Select an item.

Double click	End a mode.

Double click on
a selected object	Edit a selection.

SHIFT  single click	Extend a selection.

Right	Single click	Abort the mode.

Double click	Repeat an action.

See Also

Abort/Cancel

Selecting Objects


Editing Attributes in the Schematic Editor

Parts, ports, wires, buses and ports all have attributes associated with them.  An attribute is like a property.  It has a name and a value (which can be blank). For example, parts have attributes such as resistor values, simulation models and package types.  Wires can have attributes such as labels and trace widths.  Attribute values may or may not be displayed on the schematic.

To change the value of an attribute that is being displayed

1.	Double-click on the attribute value.

2.	Enter the new value in the Set Attribute Value dialog.  If you are changing the reference designator of a part, you will see the Edit Reference Designator dialog.

3.	Choose the OK button.

To edit the list of attributes of a selected item(s)

1.	Select the item(s)

2.	Click on the Edit Attribute button in the toolbar

or choose Attributes from the Edit Menu.

For parts, you can also simply double click on the part.

NOTE:  Changes made to attributes in the schematic editor occur on the particular part instance only.  Changes do not affect the underlying symbol in the library.

3.	To change the value of an attribute, select it from the list.  The name and value will appear in the edit fields at the top of the dialog.  Change the value in the value edit field and press the Save Attribute button.  To delete an attribute, select it from the list and press the Delete button.  To change whether the attribute name and/or value is shown on the schematic select it and press the Change Display button.  To add a new attribute, type the name and value in the edit fields and press Save Attribute.

NOTE:  Attributes marked with an '*' in the list cannot be changed in the Schematic Editor.

4 Choose the OK button to save the changes you have made.

See Also

Part Attributes

Bus Attributes

Port Attributes

Wire Attributes


Editing and Viewing Symbol Definitions
Editing and Viewing Symbols

You can easily change and/or create new symbols while in the midst of editing a schematic.  The Symbol Editor is a separate window within Schematics.  See Invoking the Symbol Editor.  If you change a symbol that is being used on a schematic that is currently displayed, the changes will take affect when you save the library.  If you create a new symbol, the library to which you save it must be one of the configured libraries in order for you to be able to use it in the Schematic Editor.

See Also

Creating New Symbols

Configuring Symbol Libraries


Modifying the Electrical Characteristics of a Part

Most parts do not permit modification of their electrical characteristics.  Breakout devices contain modifiable attributes corresponding to PSpice instance parameters.  Breakout devices are supplied for each passive PSpice primitive device (those with one of the following initial letters):

BCDJKLMQRSW

Breakout device names consist of one of these letters, plus the suffix "break."

To modify the electrical characteristics of a part:

1.	Choose Get New Part from the Draw Menu.

2.	Choose Browse to bring up the list of libraries.

3.	Select the Breakout Library to view the list of breakout devices.

4.	Select a breakout device and choose OK.

5.	The cursor changes to the shape of the part.  Place the part at the desired location on the schematic by double clicking the mouse.


Opening and Saving Schematics

To open an existing schematic:

To quickly open an existing schematic, click the Open button on the toolbar.

or choose the Open command from the File Menu

A new window will be created displaying the schematic you specified.

To save a schematic to its existing name:

To quickly save the currently active schematic with its existing name and location, click the Save button on the toolbar.

or use the Save command from the File menu.

To save a schematic to different name:

1.	Choose Save As from the File Menu.

2	Enter the name of file to which to save the schematic

3.	Choose OK.


Creating Multiple Page Schematics

In Schematics, a schematic can consist of one or more pages.  All pages are kept in the same schematic file. The Navigate menu contains the commands used to create and edit multiple page schematics.

Connections between pages are made using OFFPAGE ports of the same name.

To add another page to a schematic:

1.	Choose Create Page from the Navigate Menu.  This will create a new empty page inserted after the page you are currently editing.

2.	Use OFFPAGE ports of the same name to connect signals between pages.

To view different pages of the same schematic at the same time:

1.	Choose New from the Window Menu.  This will open a new window showing the same page of the currently active window.

2.	Choose Next, Previous or Select from the Navigate menu to display a different page in the currently active window.


Creating Hierarchical Schematics

Hierarchy in Schematics allows you to organize your design into multiple levels of schematics.  At any given level of a schematic, there can be hierarchical parts that represent other schematics.  Schematics gives supports unlimited levels of hierarchy.

Blocks and hierarchical symbols are used to represent subschematics on a page.  Each pin on the block or symbol must correspond to an INTERFACE port of the same name on the subschematic.  Connections to the pins on the block or symbol correspond to connections to these INTERFACE ports.

In Schematics, a hierarchical block or symbol can be associated with more than one subschematics by defining multiple views.

To place a hierarchical block:

1.	Choose Block from the Draw Menu.

2.	Click the mouse to place the block on the schematic.

Associating a schematic with a block:

1.	For new blocks, double-click on the block

2.	Enter the name of the subschematic in the dialog

Changing the schematic associated with a block:

1.	Choose Views from the Edit Menu.

2.	Change the schematic name shown as the Value of the Default attribute.

3.	Press OK.

To create pins on a hierarchical block:

1.	Draw a wire or bus so that it ends on the border of the block.  A dot will appear on the block signifying that a pin is created.  A default pin name will be assigned.

To edit a pin a hierarchical block:

1.	Double-click on the pin name

2.	The Change Pin dialog will appear which lets you change the name of the pin, its ERC type and other display related information.

To delete pins on a hierarchical block:

1.	Select the pin by clicking on the pin name.

2.	Press DELETE.


Configuring Symbol Libraries

To find symbols used on a schematic, Schematics searches through its list of configured libraries in the order that they are configured.  The first symbol definition it finds with the desired name is the definition that will be used when the schematic is drawn and/or netlisted.  This configured list of libraries is also the set of symbols available for use by a schematic.

When you installed Schematics, you specified the set of libraries with which to configure the editor.  These are global libraries - i.e. any schematic, new or existing, will have symbols in these libraries available.

You may also configure libraries which are local to the schematic.  I.e. configured only for that particular schematic.  Schematics always searches local libraries before searching the global libraries.

The Get Part dialog that you see when the Browse button is chosen in the Get New Part command  in the Draw Menu shows you the list of local and global libraries that are configured for the currently active schematic.  The libraries are listed in the order that they will be searched.

To Configure a Symbol Library for All Schematics

1.	Choose Editor Configuration from the Options Menu.

2.	Click the Library Settings button.

3.	Enter the name of the symbol library you want to configure.

4.	Check the Symbol box to indicate that the symbol library is to be configured

5.	Check the Package box if the library has a package library associated with it.

6.	Click the Add* button to add it as a global library (available to all schematics)

7.	Press OK.

To Configure a Symbol Library as Local:

1.	Follow steps 1-5 above.

2.	Click Add Local instead of Add*.  The library, since it is local, will appear at the top of the list.

3.	Press OK.


Using the Cut, Copy or Paste Commands

The Cut command deletes all currently selected items from the currently active schematic page and places them in the Paste buffer.  The Copy command copies selected items to the Paste buffer.  The Paste command allows you to places one or more copies of he contents of the Paste buffer onto the currently active schematic page.

There is a single Paste buffer that is shared by all schematic windows.  This allows you to Cut or Copy in one window and paste to a different window.  Thus you can easily cut/copy from one schematic to another (or one page to another page) by opening both schematics for editing at the same time.

To cut or copy an item(s) on your schematic:

1.	Select the item(s) on your schematic to be cut or copied.

2.	Choose Cut or Copy from the Edit Menu.

To paste a cut or copied item(s) onto your schematic:

1.	After cutting or copying an item(s) with the Cut or Copy commands, choose Paste from the Edit Menu.

2.	Place the cursor at the desired location for the item that was cut or copied and click left to place the item(s).  Click right to end the mode.

See Also:

Selecting Items on a Page


Using the Rewire Command

Reroutes a wire or bus segment without changing its endpoints.

To use the Rewire command:

1.	Choose Rewire from the Draw Menu.  The cursor changes to a crosshair shape.

2.	Position the cursor on the wire segment and click left.  As you move the mouse, the wire or bus segment stretches, which is shown by the cursor movement.

3.	Either click left to set a vertex, or double click to set the segment to the new routing.


Adding Text

You can add text for documentation purposes to your schematic page.  This is referred to as annotation text.

To add annotation text to your schematic

1.	Click on the Text button in the toolbar

or choose Text from the Draw Menu.

2.	Type in the desired text into the Place Text dialog.

3.	To change the size of the text, modify the Text Size shown in the dialog box to suit your needs.

4.	 Choose OK.

5.	 Move the text to the desired location on the schematic and click to place the text.  Click right to end the mode.


Creating a Schematic Page
Creating a New Schematic

To quickly create a new schematic, click the New button in the toolbar.

or choose the New command from the File Menu.

When you save your work, you will be asked for a file name to which to save your schematic.

See Also

Opening and Saving Schematics


Placing Parts

To place a part:

1.	Click on the Get New Part button in the toolbar:

or choose Get New Part from the Draw menu.

2.	Type in the name of the part if you know it and choose the OK button.  If you do not know the name of the part, choose the Browse button to see the list of configured symbol libraries and symbols.  Select a part from the list and choose the OK button.

If you cannot find the part you wish to use, you may not have configured the symbol library where it is located.  See Configuring Symbol Libraries.  An outline of the part will be shown indicating you are in place part mode.

4.	Use the mouse to position the outline at the desired location.

5.	Click to place the part..  Continue clicking to place multiple parts of that type.

6.	Right click the mouse to stop placing parts.

You can use <CTRL-R> and <CTRL-F> to rotate and/or flip the part prior to placing it.

If autonaming is enabled, parts will automatically be assigned a reference designator as they are placed.  If the part belongs to a multiple-gate package, it will be assigned to first gate of the package.

Tip:  If you already have a part of that type placed on the schematic, you can use Copy and Paste to quickly place another part of that type.  See Using Cut, Copy, and Paste.

See Also:


Placing ports
Using Ports

Ports provide a way to specify connectivity between pages and levels of hierarchy.   There are three types of ports in Schematics:  offpage, hierarchical and global.  Signals connected to ports of the same type and same name (label) will be connected together when netlisted.

Offpage ports are used to connect signals between pages of a multi-page schematic.  They may also be used to connect signals on same page without using wires.  Offpage ports only connect to other offpage ports within the same level of hierarchy.

Global ports are used to connect signals anywhere in the schematic.  I.e. signals connected to global ports of the same name on the same page, different pages, or different levels of hierarchy will be connected.

Interface ports are used to connect signals between levels of hierarchy.  Each interface port must have the same name as a pin on the hierarchical block or symbol used to represent the schematic it is on.  Thus, a signal connected to pin CLK on a block would connect to the CLK interface port on the subschematic.

Ports in Schematics are a type of symbol and have a single pin. The type of port a symbol represents, offpage, global or interface, is defined by the symbols type.

To place a port on your schematic

1.	Click on the Get New Part button in the toolbar:

or choose Get New Part from the Draw menu.

2.	Type in the name of the part if you know it and choose the OK button.  If you do not know t the name of the part, choose the Browse button to see the list of configured symbol libraries and symbols.  The library port.slb has ports that come with Schematics.  Select a part from the list and choose the OK button.

3.	An outline of the part will be shown indicating you are in place port mode.

4.	Use the mouse to position the outline at the desired location.

5.	Click to place the port..  Continue clicking to place multiple ports of that type.

6.	Right click the mouse to stop placing parts.

Schematics provides a set of commonly used port symbols in port.slb.  You may also create your own using the symbol editor.

To label a port

1,	Double-click on the port.

2.	Enter the port label in the Set Attribute dialog.

3.	Choose the OK button.

Ports may connect to wires, busses or directly to other part or port pins. The label of the port determines the number of signals it represents.  Its format is the same as that of wires and buses.  See Labeling Wires, Buses and Ports.. Examples of valid port labels are:

INPUT

CLK[0-15]

CLK[0:15]

CLK[0..15]

See Also:

Placing Parts


Drawing Wires and Buses

Wires and buses are used to represent electrical connections between pins.  A wire represents a single signal while buses represent multiple signals.

Wires and buses are composed of one or more connected segments.  If you have orthogonal enabled in the Display Options dialog, segments will be drawn orthogonally (perpendicular to each other).  If turned off, wires and buses can be drawn at any angle.

Junction dots will appear wherever three or more pins, wire or bus segments meet and indicate connectivity. These junction dots are created and removed automatically by Schematics.

If a wire crosses another wire, they are connected only if there is a junction dot at the intersection.  This will happen only if, while drawing the second wire, you end a segment on the other wire by clicking then continue the wire..

To draw a wire:

1.	Click on the Draw Wire button in the toolbar or choose Wire from the Draw Menu.

The mouse cursor will change to the outline of a pencil indicating that you are in wiring mode.

2.	Click the mouse at the point at which you want to start the wire.

3.	Click the mouse to create consecutive segments.  If you click on a pin or the midpoint of another bus or wire, the wire will be ended and you will be left ready to start a new wire.

To draw a bus:

1.	Click on the Draw Bus button in the toolbar or choose Bus from the Draw Menu.

The mouse cursor will change to the outline of a pencil indicating that you are in bus drawing mode.

2.	Click the mouse at the point at which you want to start the bus.

3.	Click the mouse to create consecutive segments.  If you click on a pin or the midpoint of another bus or wire, the bus will be ended and you will be left ready to start a new bus.

See Also:

Labeling Wires, Buses, and Ports

Connecting Wires to Buses


Connecting Wires and Buses

Wires connect directly to buses without any special handling. The wire must be labeled with one of the signals of which the bus is comprised. This label is what defines the connectivity between the bus and the wire.

To connect a wire to a bus:

1.	Draw the wire so that one end falls on the bus.  A junction dot should appear indicating that the wire is connected to the bus.

2.	Label the wire with one of the signals represented by the bus.  E.g. if the bus is labeled A[0:2], the wire can be labeled A[0], A[1], or A[2].

To connect a sub-bus to a bus:

1.	Draw the subbus so that one end falls on the bus.  A junction dot should appear indicating that the wire is connected to the bus.

2.	Label the subbus with one of the signals in the main bus.  E.g. if the bus is labeled A[0:15], the subbus can be labeled A[0:7].

See Also:

Labeling Wires, Buses, and Ports


Connecting to Power and Ground

Placing Power and Ground Symbols on Your Schematic

Power supply and ground symbols are represented by global port symbols in Schematics.  The label on the port defines the name of the power supply or type of ground.

The port.slb symbol library shipped with Schematics contains some common ground symbols and a global port symbol pre-labeled 5V.  You can use this 5V symbol for any power supply by placing it and changing the label

See Also:

Using Ports


Adding Text to a Schematic

Annotation text can be added to a schematic page with the Text command in the Draw Menu.  This text is for documentation purposes only; it is ignored by the netlister.  Once you have placed text on the schematic, you can change the text and/or its size by double-clicking on it.  You can turn off and on the display of the text by enabling/disabling User Text 1 in the Set Display Level dialog.


Labeling Wires, Buses and Ports

Labels are used to define a signal name on a wire or port, or a set of signal names on a bus.

To label a wire, bus or port

1.	Double-click on a wire, bus segment or port

or

Click on the wire segment, bus segment or port to select it and choose Label from the Edit Menu.

2.	Enter the label name in the Set Attribute dialog.

3.	Choose the OK button

A wire or bus has a single label or name associated with it.  However, you can have the label shown multiple times (once per segment) by double-clicking on each segment and press OK to the Set Attribute dialog that displays the label.  Note that changing the label on one segment will change it for all segments.

Bus Labels

Bus labels define the set of signals that the bus represents.  To specify a range, the label may be of the form:

busname[n..m]	e.g. CLK[0..5]

busname[n:m]	e.g. CLK[0:5]

busname[n-m]	e.g. CLK[0-5]

where busname is the name of the bus and n-m represents the range of the wires of the bus.  Wires connected to the bus would have labels such as CLK0, CLK1, CLK2 or CLK[0], CLK[1] or CLK[2] ([] are optional for wire labels.

The bus label may also be a comma separated list of signals:

name,name1,name2	e.g. CLK0, CLK1, DATA

Ports that are connected to buses would have labels of the same format as a bus.

See Also:

Connecting Wires and Buses


Panning and Zooming

Panning (autoscrolling)

If the Autopanning option is enabled, Schematics will automatically scroll the window when the cursor is left in the hot zone along the windows borders for a certain period of time.  (The cursor will change to a solid arrow when in the hot zone).  If autopanning is disabled, you must use the scroll bars to scroll the window.  Use the Pan & Zoom command in the Options Menu to change the size and sensitivity of the hot zone.

Zooming

Schematics support unlimited zooming.  You can specify the factor at which you zoom in and out using the View commands with the Pan & Zoomcommand in the Options Menu.

To Quickly Zoom In or Out on the currently active page

1.	Click the View In button in the toolbar

to increase the magnification, or click the View Out button

to decrease the magnification by the amount specified in the Pan & Zoom dialog.

The same center point will be kept.

To Zoom In or Out on your Schematic with a new center point

1.	Choose In or Out from the View Menu.

2.	Click at the point you want centered.

3.	The magnification will increase or decrease by the amount set in the Pan & Zoom dialog with the point you chose centered in the window.

Tip
You can zoom in or out while in the midst of placing parts and wires by using <CTRL-I> (for In) or <CTRL-O> (for out)

To Zoom In on a Particular Area on your Schematic

1.	Click the View Area button in the toolbar

or choose Area from the View Menu.

2.	Draw a box around the area you want to zoom in on.

3.	The magnification will be increased so that the area you selected is visible in the window without changing the aspect ratio.

See Also:


Using the View Menus
Using the View Menu

Choose from the following items on the View Menu to change the viewing scale on your schematic:

Menu Item	Function

Fit	Resets the viewing scale so that all parts, wires and text can be seen.

In	Allows you to view an area on the schematic at closer range (i.e., to magnify).

After selecting this item, a crosshair appears.   Move the crosshair to the area on which you want to zoom in.

Out	Changes the viewing scale so that you can view the schematic at a greater distance away (i.e., to view more of the schematic on the screen).

After selecting this item, a crosshair appears.  Move the crosshair to define the center of the viewing area.

Area	Allows you to select a rectangular area on your schematic to be expanded to fill the screen.

If you already have a selection box on your screen when you choose Area, the contents of the selection box will be expanded.

Or, drag the mouse to form a selection box around the portion of the schematic you want to have expanded.  The items contained within the selection box will be expanded to fill the screen.

Entire Page	Allows you to view the entire schematic page at once.


Invoking the Symbol Editor from the Schematic Ediotr
Invoking the Symbol Editor from the Schematic Editor

You can invoke the symbol editor from the schematic editor by using either of the commands shown below:

Using the Edit/Symbol Command:

1.	Select a symbol on your schematic to edit.

2.	Choose Symbol from the Edit Menu

3.	The symbol appears in a new window in the symbol editor, ready for editing.  The menu bar also changes to that of the symbol editor.

4.	After editing the symbol, you must save the changes for it to affect the schematics that use that symbol.

Using the Edit Library Command:

1.	Choose Edit Library from the File Menu.

2.	The symbol editor menu appears, and you are ready to select a library to edit or to create a new one.

3.	Choose Exit from the File Menu to return to your schematic.


Creating Symbol Graphics

From the symbol editor, you can create new graphic elements for symbols.

Drawing Arcs

1.	Choose Arc from the Graphics Menu.  The cursor changes to a pencil shape.

2.	Click left to select one end point of the arc on the schematic.   Click again to select the other end point.

3.	As you move the mouse, you will see the changing shape of the arc.

4.	When the arc is the desired size, click left to fix the arc.

Drawing Boxes

1.	Choose Box from the Graphics Menu.  The cursor changes to a pencil shape.

2.	Click left to select a location for the corner of the box on the schematic.

3.	As you move the mouse, the cursor is attached to the opposite corner of the box, and the corresponding box is shown.

4.	When the box is the desired size, click left to fix the box.

Drawing Circles

1.	Choose Circle from the Graphics Menu.  The cursor changes to a pencil shape.

2.	Click left to select the center of the circle on the schematic.  Then move the mouse to extend the diameter of the circle.

3.	Click left to set the circle at the desired size.

Drawing Lines

1.	Choose Line from the Graphics Menu.  The cursor changes to a pencil shape.

2.	Click left at the starting point for the line on the schematic.

3.	Move the cursor to extend the line.

4.	Click left to set a vertex, or double click to end the line.

Drawing Pins

1.	Choose Pin from the Graphics Menu.  The Add Pin dialog box appears.  You can change the Name, the Pin Number, or the ERC attribute.  Or, choose OK to place a pin with the same characteristics as the previously placed instance of that pin.

2.	Move the pin outline to the desired location and click left to place the pin.  A small "x" appears to mark the connection point of the pin.

3.	The Add Pin dialog box appears after adding a pin.  You can add additional pins by clicking the mouse at the desired location.

4.	Double click to place the current pin and end the mode.  Or, click right to end the mode without placing the current pin.

NOTE  Prior to selecting the location for the pin, you can use the Flip (CTRL+F), Rotate (CTRL+R), or Pin Type (CTRL+T) commands from the Edit Menu to change the display of the pin.

See Also

Changing the Pin Type


Creating New Symbols

You can create a new symbol either from scratch, or by importing the characteristics of another symbol.

To create a new symbol:

1.	Choose Definition from the symbol editor Part Menu to bring up the Definition dialog box.  You can enter the following information:

Description	The textual description of the symbol.

Part Name	The most commonly used full name of the part.  This name, or an alias, is the name that will be used to create netlists and to bring an instance of the part into the schematic.

Alias List	The exact electrical equivalents of the part that can be used to reference the symbol.

AKO Name	If a symbol contains an AKO Name, it means that it will use the graphics, pins, and attributes of the named part.  Attributes on the original symbol will be overridden by those from the new symbol, and new attributes may be added.

If graphics and/or pins already exist for the symbol, you will be prompted to verify whether you want them replaced with those of the symbol referred to in the AKO.  For symbols specifying an AKO, the following rules apply:

The symbol it refers to must reside in the same library.

You can only edit the attributes and the definition.

Type	Symbol types include:  primitive, port, annotation, border, or title block.  Only primitive and port symbols contain electrical properties.  Annotation, border, and title block symbols have no electrical significance.

NOTE:  Choose Copy from the Edit Menu to copy an entire symbol with its pins and graphics to a new part name.

2.	Define the attributes for the part by choosing Attributes from the Part Menu.  The dialog box fields are explained under Editing Attributes in the Symbol Editor.

3.	Choose Add or Delete at the bottom of the dialog box to add or delete the symbol from the list.  Choose OK to initiate the action, or Cancel to abort.

See Also

Editing Attributes in the Symbol Editor

Editing and Viewing Symbol Definitions

Adding Symbol Graphics


Editing Attributes in the Symbol Editor

In the symbol editor you can define new part attributes or modify existing attributes.  You can also change any system attribute value or add new attributes.  (System attributes are those attributes that are required for netlisting to PSpice/PLogic, are used in the title block, or are used in the Special Symbols.)

NOTE:  Changes made to symbols in the symbol editor have a global implication.  All changes to parts in the libraries will affect all instances of such parts.

To edit an attribute, use method A, B, or C below:

A.	Choose Attributes from the Part Menu to bring up the Attributes dialog box.  Select an attribute to modify from the list that appears.  If a new name is added under the Name item, and it does not match any other name in the list of items at the right of the dialog box, a new attribute will be added to the attribute list.

B.	Double click on a part attribute to bring up the Change Attribute dialog box.  This dialog box allows you to edit all aspects of a particular part, but it does not add new attributes to the list.

C.	Double click on a pin attribute to bring up the Change Pin dialog box.  You can change the value of the Pin or ERC attributes, or click on the Edit Attributes button to bring up the Attributes dialog box containing the attributes for that pin.  (Refer to Changing Pin Attributes.)

Attributes or Change Attribute Dialog Box Fields

Field Name	Description

Name	Specifies the attribute name.  If the name of the attribute is the same as that of another part in the list, the part in the list will simply be modified.

Value	Specifies the attribute value.

Changeable in Schematic	Determines whether the attribute can be edited in the schematic editor.

Keep Relative Orientation	Specifies whether the attribute text will be rotated when the symbol is rotated in the Schematic Editor.

Display Value	Specifies whether or not the attribute value will be shown on the schematic.

Display Name	Specifies whether or not the name will be shown on the schematic.

Layer	Specifies the display layer for the attribute text.

Size, Orient., Hjust, Vjust	Sets the size, orientation, and justification for pins.

When you are satisfied with your changes, click on one of the following buttons:  OK or Cancel for the Change Attribute dialog box, or on one of the following for the Attributes dialog box:

OK	Incorporates the changes made to the list of attributes for a particular part.

Cancel	Aborts the session with no change.

Save Attr	Temporarily incorporates your changes to the list of attributes for a particular part.

Del Attr	Deletes an attribute from the list.  Either select the attribute from the list or type in the name of the attribute you wish to delete and click on this button.

See Also

Changing the Pin Type


Changing the Pin Type

The Pin Type command acts as a toggle to set the default pin display type for selected pins.  Seven types of pins are available.

To change the pin type, use either method A or B below:

A.	Select the pin(s) on the symbol for which you want to change the display type.  Choose Pin Type from the Edit Menu to cause each selected pin to advance to the next display type.

B.	Double click on the selected pin to bring up the Change Pin dialog box, in which you can modify the following:

Pin Name	Defines the number of signals that must be contained in a connecting wire or bus.  The naming format is as follows:

Within square brackets, use commas to separate individual members of a bus.

A dash indicates a range.

Outside of square brackets, commas separate signal names or buses.

Type	Determines how the pin will be displayed.

Hidden	Allows you to set a pin to be invisible in the schematic editor.  If you set the visibility off, you must supply the name of a connecting node for this pin.  This node is recorded as a symbol attribute (not a pin attribute).  The IPIN (pin name)=net name attribute conveys the net name.

Net	Specifies the name of the net to which a hidden pin will be connected in the schematic editor.  Enter the name of the connecting node in the Net field.

Size, Orient.,Hjust, Vjust	Sets the size, orientation, and justification for pins.

Under Pin Attributes in the dialog box, you can set the following:

Pin	Sets the pin number.

ERC	Sets the electrical type for the pin (used when the Electrical Rule Check command is applied).

Float	Specifies what the netlister should do with the pin if the pin is left unconnected:  treat as an error (must be connected),  attach a large resistor to ground (for analog pins), or allow to float.

Modeled	Specifies whether the pin is modeled in its simulation model.

Edit Attributes	Allows you to edit all pin attributes in more detail.

See Also

Editing Pin Attributes


Adding New Attributes

Attributes are special characteristics (a name and an associated value) contained in a part instance or definition.

To add a new attribute:

1.	Choose Attributes from the Part Menu.

2.	Enter the name for the new attribute in the dialog box.

3.	Modify any of the edit fields if desired.  The edit fields are described under Editing Attributes in the Symbol Editor.

NOTE:  If you change the Name, the new attribute will be added to the list, and the old one will remain unchanged.

4.	Choose from the following items in the dialog box:

OK	Incorporates the changes.

Cancel	Aborts the session with no change.

Save Attr	Incorporates your changes to the list of attributes for a particular part.

Del Attr	Deletes an attribute from the list.  Either select the attribute from the list or type in the name of the attribute you wish to delete and click on this button.

See Also

Editing Attributes in the Symbol Editor


Adding New Pins

Allows you to add new pins to a symbol.  Prior to adding a pin(s), if no pins are selected on the schematic, you can define the pin type with the Pin Type command on the Edit Menu.

To add a new pin:

1.	Choose Pin List from the Part Menu.

NOTE:  If you change the name of the pin, the new pin will be added to the list, and the old one will remain unchanged.

2.	The Pin List dialog box appears, in which you can modify the following:

Pin Name	Defines the number of signals that must be contained in a connecting wire or bus.  The naming format is as follows:

Within square brackets, use commas to separate individual members of a bus.

A dash indicates a range.

Outside of square brackets, commas separate signal names or buses.

Type	Determines how the pin will be displayed.  Seven display types are available.

Display Name	Specifies whether or not the Pin Name will be displayed on the schematic.

Size, Orient.,Hjust, Vjust	Sets the size, orientation, and justification for pins.

Hidden	Allows you to set a pin to be invisible in the schematic editor.  If you set the visibility off, you must supply the name of a connecting node for this pin in the Net field.  This node is recorded as a symbol attribute (not a pin attribute).

Net	Specifies the name of the net to which a hidden pin will be connected in the schematic editor.  Enter the name of the connecting node.  The IPIN(pin name)=net name attribute conveys the net name.

Under Pin Attributes in the dialog box, you can set the following:

Pin	Sets the pin number.

ERC	Sets the electrical type for the pin (used when the Electrical Rule Check command is applied.

Float	Specifies what the netlister should do with the pin if the pin is left unconnected:  treat as an error (must be connected),  attach a large resistor to ground (for analog pins), or allow to float.

Modeled	Specifies whether the pin is modeled in its simulation model.

Edit Attributes	Allows you to edit all pin attributes in more detail through the Attributes dialog box.

3.	Choose from the following items in the dialog box:

OK	Incorporates the changes.

Cancel	Aborts the session with no change.

Save Pin	Incorporates your changes to the list of attributes for a particular part.

Del Pin	Deletes an attribute from the list.  Either select the attribute from the list or type in the name of the attribute you wish to delete and click on this button.

See Also

Editing Pins


Editing Pin Attributes

You can edit pin attributes or add new attributes to the list.

To edit pin attributes:

1.	Select the pin for which you want to edit the attributes.

2.	Choose Change from the Edit Menu.

3.	When the Change Pin dialog box appears, click on the Edit Attributes button in the dialog box.

4.	An Attributes dialog box appears, in which you can edit the attributes for the pin(s).  Changing the Name field adds a new attribute to the list.

5.	In this dialog box, you can also determine the relative font size for the text, the orientation, and its horizontal or vertical justification.

See Also

Editing Pins


Editing Pins

You can edit all pins in a part with the Pin List dialog box.  The fields in this dialog box are described under "Adding New Pins."

To edit pins:

1.	Choose the Pin List command from the Part Menu.

2.	Select a pin to modify in the Pin List dialog box.

3.	Modify the desired fields.

4.	Choose from the following:  Save Pin, Delete Pin, OK, or Cancel.

See Also

Adding New Pins

Editing Pin Attributes


Changing the Origin of a Symbol

When you place a part, or substitute one part for another part, the part is placed according to its point of origin, or reference point.  The default reference point is shown by a small square on the part.

To change the origin:

1.	Choose Origin from the Graphics Menu.  The cursor is replaced with a pencil shape.

2.	Move the pencil to the new location for the reference point, and click left to fix the point of origin.


Resizing the Bounding Box

The bounding box surrounds a symbol, and may be resized.

To resize the bounding box:

1.	Choose BBox from the Graphics Menu.  The cursor is replaced with a pencil shape.

2.	Click left to attach the cursor to the right corner of the bounding box.  (All of the graphics and pins for the symbol must be contained within the bounding box.)

3.	Resize the box by selecting a new location for the right corner of the box and clicking the mouse at the new location.


Annotating Your Schematic

Assigns a unique reference designator for parts in the current schematic.  All parts must have a reference designator assigned before generating a netlist.

To annotate your schematic:

1.	Choose Annotate from the Analysis Menu to create a unique reference designator for parts in the current schematic.

2.	In the dialog box, choose whether to label only unlabeled parts, renumber all automatically annotated parts, or to renumber all annotated parts.

3.	Choose OK.

4.	Turn on (enable) the Auto-Naming function from the Options Menu if you wish to automatically create reference designators as you place parts.


Creating a PSpice/PLogic Netlist

A simulation netlist provides the circuit definition and connectivity information in PSpice/PLogic netlist format.

To create a PSpice/PLogic netlist:

Choose Create Netlist from the Analysis Menu.  All buses, connectors, etc. will be resolved into nodes.

Several files will be created:

file.net	contains the netlist

file.cir	contains simulation commands

file.als	contains signal name alias information


Performing an Electrical Rule Check

The Electrical Rule Check command performs an electrical check of the schematic.  This command checks the connections on the schematic for floating pins, duplicate labels, etc.

To perform an Electrical Rule Check of your schematic:

1.	Choose Electrical Rule Check from the Analysis Menu.

2.	If a message on your screen indicates that errors are present, choose Current Errors from the Analysis Menu to view the errors.


Running a PSpice Simulation
Running a Simulation

PSpice/PLogic produces a circuit analysis on the current schematic.  Running the simulator automatically performs the following (if necessary):  annotation, electrical rule check (ERC), and netlist generation.

To run a simulation:

1.	Choose the analyses you wish to perform on your circuit by selecting from the Setup options on the Analysis Menu.

2.	Verify that you have executed the following three commands from the Analysis Menu:

Annotate

Electrical Rule Check

Create Netlist

3.	Choose Current Errors, if a message appears that errors are present.

4.	Choose Simulate from the Analysis Menu (or use the F11 function key).

5.	Choose Examine Output to view the bias point information, model parameter values, simulation errors, etc. in the form of a text file.

See Also

Annotating Your Schematic

Performing an Electrical Rule Check

Creating a PSpice/PLogic Netlist


Specifying Output Variables

Certain analyses require you to specify "output variables" for voltages and currents at specific points on the schematic.  You can specify the voltage or current at a pin, at a terminal of a semiconductor device, or through a part.  Some analyses require only a device name.

To specify output variables:

1.	Choose Setup from the Analysis Menu.

2.	As you choose the analyses to perform on your circuit from the choices presented, determine if the analysis type requires you to enter an output variable in the dialog box:

(e. g., AC Sweep and Noise, and Monte Carlo require output variables).

3.	In the dialog box for the analysis type, specify the voltage or current in the following format:

v(<fully qualified pin name>) as in v(R1:1)

i(<device>) as in i(R2)

If desired, specify the relative voltages between two different pins using the V(a, b) notation, where a and b are the positive and negative pins.

To specify the voltage or current at a terminal of a semiconductor device:

Assign a terminal identifier suffix (such as "C" for collector) to the V (voltage) or I (current).

For example:  VC(Q3) or IC(Q3)

To specify the current through a part, use the following notation:

I(R23)


Using Special Symbols to Setup SimulationsCommands
Using Special Symbols to Setup Simulation Commands

Special symbols enable you to interact with the circuit simulation by placing symbols on the schematic that act in the same way as PSpice/PLogic command lines in the circuit file.

Analog Stimulus Symbols

Analog stimulus symbols are PSpice independent voltage sources (V devices) and current sources (I devices).  There are five variants which correspond to the transient specifications available in PSpice:  PWL, SIN, EXP, PULSE, and SFFM.  The symbol type is indicated by a V or I, followed by the transient specification name.

Digital Stimulus Symbols

Digital stimulus symbols are PSpice/PLogic file stimulus devices used to obtain digital stimuli from an external file.

Setpoints

Setpoints specify nodeset or initial condition voltages.  Setpoint symbols consist of the following:  ic1, ic2, nodeset1, or nodeset2 (with one or two pins).  After placing a setpoint symbol, connect up the pins.

Viewpoints

Viewpoints display bias point voltage and currents.  Viewpoint symbols consist of the following:  vpoint and isensor.  After placing a viewpoint symbol, connect up the pins.

To place special symbols:

1 Choose Get New Part from the Edit Menu to bring up the Special library.

2 Select a part to place on your schematic from the list displayed.


Using Probe

Probe is MicroSim's waveform analyzer, which you can use to view simulation results.  A successfully completed simulation produces a .dat file, which contains the simulation results necessary for creating a Probe display.

To use Probe:

Choose Run Probe from the Analysis Menu (or use the F12 function key).


Modifying the Libraries
Modifying the Model Library List

To modify the libraries:

1 Choose Library and Include Files from the Analysis Menu.

2 Edit the list of library and include files.  You may add, remove, or change a library from the set of libraries in msim.ini or the set local to the current schematic.

3 Choose OK to confirm the action.

See Also

Library and Include Files


Setting the Search Path for Libraries

The library search path contains the directory or directories which contain symbol, package, and simulation model libraries.

To set the library path:

1 Choose Editor Configuration from the Options Menu.

2 In the dialog box, modify the library path to suit your needs.  Changes to the path will take effect the next time Schematics is restarted.


Printing a Schematic

You can print one or more pages of the current schematic.

To print a schematic:

1.	Choose Print from the File Menu.

2.	Select the page(s) you want to print.

3.	Or choose All (or None) to print (not print) the pages.

4.	Choose OK.

See Also

Printer Setup


Printing a Symbol

In the symbol editor, you can print a copy of the current symbol or desired symbols in the current directory.

To print a symbol:

1.	Choose Print from the File Menu.

2.	In the dialog box, choose whether you want to print the current symbol only.  If so, click left on Current Symbol Only to enable the function.  If you want to print multiple parts, click left to disable Current Symbol Only, and choose the symbols you wish to print from the list on the left.

3.	Or, use the following fields, as desired:

Select All Parts	Prints all parts in the current library.

Clear Selections	Clears any parts you may have selected from the list.

Symbol Image	Prints the symbol graphics.

Symbol Data	Prints the symbol definition as shown in the Definition dialog box on the Part Menu.

Attributes	Prints the symbol attributes as shown in the Attributes dialog box on the Part Menu.

Pin Data	Prints the information appearing in the Pin List dialog box on the Part Menu for the Pin Number and the ERC only.

Auto-Fit	Fits one symbol on the printer page.

User-Definable Zoom Factor	At the 200% (default) setting, symbols will always be printed in constant relation to each other.  It is advisable to leave this feature set at the default, unless you want to print an enlarged (or smaller) image of a symbol.

See Also

Auto-Fit


Printer Setup

Allows you to set up various printer options, such as landscape or portrait mode, paper size, and printing resolution.

To set up the printer:

1.	Choose Printer Setup  from the File Menu.

2.	In the dialog box, select the printer you will be using, and select from the other options shown to set up your printer to suit your needs.

3.	Choose OK.


Setting Auto-fit

Auto-fit automatically sizes your schematic so that it will fit on one piece of printer paper.

To set Auto-fit:

1 Choose Print from the File Menu.

2 Then choose Auto-fit in the dialog box and select OK.


Setting the User-Definable Zoom Factor

The User-definable zoom factor allows you to enter a percentage in the dialog box, which determines the number of printer pages needed to print a particular schematic.

To set the User-definable zoom factor:

1.	Choose Print from the File Menu; then choose User-definable zoom factor in the dialog box.

2.	Enter a value (in percentage) for the zoom factor, depending on the size of your schematic page and the size of printer paper you are using.

Doubling the zoom factor quadruples the number of printer pages needed to print a schematic.

Using a zoom factor of less than 100% reduces the number of printer pages needed.


Selecting Objects
Selecting Items on a Schematic

In general, you must select items on your schematic in order to move, delete, copy or edit them.  You can select individual parts, ports, wire segments, bus segments and annotation text.  You may also select individual attributes, such as reference designators and port labels.

When an item is selected, it will be drawn in red (or the configured selection color) indicating it is selected.  If you have selected an attribute, such as the reference designator or label, a box will be drawn around the text indicating it is selected.  A dashed box will be drawn around the part, port, wire or bus segment which owns the attribute.

To select a single item

1.	Click the left mouse button on the item (e.g. part or wire).

To select a group of items

You can select a group of objects by using a selection area.  Any items wholly within the area will be selected.

1.	Hold down the left mouse button while "dragging" the mouse across the area you wish to select.  Release the mouse button to end the area.  A "selection box" appears on your screen, and all items within it are selected.

Note that attribute text cannot be selected using selection areas.

To select/deselect additional items

1.	Hold down the SHIFT key while selecting additional items.  SHIFTClick on a selected item will deselect it.

You can also use the Find command to select items.


Moving Parts, Wires and Text

To move items on the page

To move items on the schematic, such as parts, wire segments, bus segments and text, you must first select the items to be moved.  Selected objects may be moved by simply dragging them to a new location on the schematic page, as follows:

1.	Select the items to be moved by clicking on it or drawing a selection area.  See Selecting Items on a page,

2.	Position the mouse cursor on the selected item(s) and hold down the left mouse button.

3.	Drag the selected item(s) to the desired location

4.	Release the mouse button

If rubberbanding is enabled, connectivity will be maintained by insertion of additional wire and bus segments.  To enable rubberbanding, press F8.  To disable it, press <SHIFT>F8 or use the Display Options command in the Options menu.

See Also

Selecting Items on a Page


Abort/Cancel

Cancels the current action.

Use any of the three methods below to abort or cancel the current action:

1.	Press the Esc key.

2.	Choose Cancel from the dialog box, where applicable.

3.	Press the right mouse button.


Bus Attributes

Each bus must have an associated label attribute in order for the circuit to be netlisted.  Each wire connected to the bus must also have a label, which establishes it as a component of a specific bus.

Label	Specifies the signals that make up the bus.

See Also:

Labeling Wires, Buses, and Ports


Port Attributes

Port attributes consist of the following:

Label	The most significant attribute of a port is the Label.  A connection occurs when two global ports have the same Label attribute value anywhere in the design.

If an offpage port contains a Label attribute and the wire or bus attached to it also contains a Label attribute, the Label attribute values must be identical to be acceptable for netlisting.

See Also:

Labeling Wires, Buses, and Ports


Part Attributes

Part attributes consist of the following:

Refdes	Consists of the PKGREF and GATE attribute values to uniquely identify a part.  This attribute cannot be changed directly.  To change it, change the PKGREF and/or GATE attribute.

PkgRef	The reference designator for the part

Gate	Gate name within the package

Part	The name of the symbol used when Get New Part was done to place an instance on the schematic.

Template	Defines how to netlist the part for simulation (optional)

User-Defined Attributes	Additional attributes defined by the user when the symbol was created.


Wire Attributes

Wire attributes consist only of a Label.  If a wire is connected to a bus it must  have a Label, which establishes it as a component of a specific bus.  Otherwise, a Label is optional.

See Also:

Labeling Wires, Buses, and Ports


Packaging
Packaging a Schematic

Packaging is the process of collecting individual gates into physical packages and reassigning reference designators and gate names to replace how they are package.  The packager uses package definitions contained in the package libraries (.plb).  Package definitions contain information about the number of gates per package, gate names and pin numbers for the different gates.

To package your schematic, use the Annotate in the Tools Menu with the Package and Assign Reference Designators option enabled.


Manually assigning gates;reference designators
Manually Assigning Reference Designators and Gates

To assign a specific reference designator and/or gate to a part on the schematic, double-click on the reference designator that is displayed.   This brings up the Edit Reference Designator dialog which lets you change the reference designator and/or the gate to which the part is assigned.

For example, create a new schematic (File/New), and place a 7404 down on the page (Draw/Get Part).  You should see U1A displayed by the part.  This is the reference designator and gate that are automatically assigned to the part as you place it.  To change the gate to B,  double-click on the text U1A, change the A to B, the press OK.  You should now see that U1B is displayed.

When you package the schematic, be sure the All Except User-Assigned or the Only Unassigned option is enabled so that the packager does not reassign reference designators and gates to those parts you have explicitly assigned.


Generating a Bill of Materials Report

Use the File/Reports/Bill of Materials to generate a Bill of Materials report either to the screen, the printer or to a file.  The information included in the Bill of Materials for each part is configurable via the File/Reports/Report Setup dialog.  You can also include part information from an external database by generating a file in a standard database format and configuring Schematics to use this information.  See....


Choosing a layout netlist format

Use the File/Reports/Bill of Materials to generate a Bill of Materials report either to the screen, the printer or to a file.  The information included in the Bill of Materials for each part is configurable via the File/Reports/Report Setup dialog.  You can also include part information from an external database by generating a file in a standard database format and configuring Schematics to use this information.  See....


Creating a Layout Netlist

The Tools/Create Layout Netlist will generate a layout netlist file in the currently configured format.   The netlist file will be created in the same directory as the schematic and be named <schematic name>.<default extension> where the <default extension> can be changed with the Tools/Configure Layout Editor command.

If you have not run the Tools/Annotate command and packaged your schematic, you will get a message Warning:  the schematic has not been packaged.  Continue?.  While it is not required that you package the schematic, it is highly recommended.  Packaging creates a cross-reference file that allows you to later backannotate ECO changes from the layout editor.  If packaging is not done, back annotation will not be possible.  Also, packaging will ensure that all parts have been assigned reference designators and package types (footprints).

SideBar:  Schematics uses mapping file which defines the rules used to generate the partlist entries for different part types in the layout netlist.   You may have to add entries to this file (using a text editor) if you have parts which do not follow the default format.  There are also mapping files for translating package type names (footprints) into the names that the layout editor uses (e.g. DIP-8 vs. DIP8)


Defining Package Information

As mentioned previously, the packaging process using package definitions to obtain information such as the number of gates per package, gate names, in which footprints the part is available and the pin numbers for the pins.   When creating new symbols, you should create a corresponding package definition, using the Packaging/Edit command in the Symbol Editor,  which defines:

.	the package types (footprints) in which the part is available

.	the number of gates per package

.	the pin number assignments for each pin for each gate

.	which pins within a gate are swappable

.	which pins are shared (power and ground usually) between gates

If you do not create a package definition for a symbol, it is assumed that it has only one gate per package, will have no footprint associated with it, and will use the pin numbers defined for the symbol.


Model Editing

The Edit Model dialog will give you the choice of changing the name of the model referenced by the selected part, or editing an instance model (a copy) of the part.  The Change Model Reference button brings up a dialog that allows you to enter the name of another model or subcircuit for this part instance.  The Edit Instance Model button allows you to edit a copy of the model or subcircuit definition.  If an instance model does not already exist, the Schematic Editor creates a new instance model definition that is a copy of the original model.

See Also

Using the Model Editor


Using the Model Editor

The Model Editor dialog is a mini-text editor that allows you to edit the model or subcircuit definition of a part.  If you are editing a model definition, then the text field will contain one parameter per line.  All of the comments immediately before or after the model or subcircuit definition are included for editing.  Note that this will sometimes mean that comments intended for the previous or next model definition will be included in the edit dialog.

The Expand AKO command will search through any AKOs that the model might have, adding the new parameters to this model.  In essence, this command "flattens" a hierarchy of AKOs into one model where you can see all the parameters.

Notes on Editing within Microsoft Windows.

The editor follows the Microsoft Windows default dialog and edit field conventions. The following accelerator keys may be used.

Key	Action

ENTER	Insert newline

CTRLX	Cut

CTRLC	Copy

CTRLV	Paste

CTRLZ	Undo/Redo

CTRLTAB	Insert tab

The TAB key by itself will move focus to the next field in the dialog.


Library and Include Files

This dialog allows you to edit the list of library and include files that Schematics will insert in the netlist that it sends to the simulator.  The files marked with an "*" are from the [SCHEMATICS NETLIST] section of the "msim.ini" file.  These files are included in every netlist created by Schematics.  The other files (if any) are local to the schematic presently being edited.  This permits you to customize the library and include files put in the netlist for any particular schematic.

Note that the "local" library and include files will always be included in the netlist before the "global" files from "msim.ini".  This means that if you have a model in a local library file that has a name identical to one found in a file from "msim.ini", the local model name will always be found first.

When you edit or create new model or subcircuit definitions using the built-in model editor, the library file created will automatically be put in the library and include files list as a local library.

New library or include file names may be added to either "msim.ini" or the local schematic list be typing their name in the <File Name:> edit field.  The <Add Library> or <Add Include> command adds the file to the local list, the <Add Library*> or <Add Include*> command will add the file to "msim.ini".  The <Delete> command deletes the file currently selected in one of the lists (only one file can be selected at any time).  The <Change> command deletes the selected file from the list and pastes it in the <File Name:> edit field, to be modified and/or inserted back in a list.  The <Find...> command will allow you to browse through the directory structure looking for file names.  If a file name is selected it will be pasted in the <File Name:> edit field when you return to the Library and Include Files dialog.


Polaris

Before invoking the extractor, you must set up the parameters that Polaris uses to determine how it will extract transmission lines and compute the coupling between the extracted lines.

The options to set up, run, and simulate using Polaris are accessible through this dialog.

Basic Steps for extracting PCB Layouts:

Before invoking Polaris, you must do the following:

1.	Capture your schematic using Schematics, package the components by enabling Package and Assign Reference Designators under Analysis/Annotate, and generate a layout netlist using Tools/Create Layout Netlist.  This netlist file, or "NONE" is shown in the top of the dialog.

2.	Create a routed layout for the board.  Polaris supports PADSASCII, PCAD PDIF, and RacalRedac CADStar layout formats.  In order to use Polaris, the layout must have been created from a netlist generated by Schematics.  The routed layout file name (specified in Polaris setup), or "NONE", is shown below the netlist file.

3.	Specify the nets to be extracted by attaching a Polaris marker to one of the device pins attached to the desired net or anywhere on the net.  Polaris markers are similar to Probe markers except that their function is only to mark signals for extraction.  An alternative is to select all (routed) nets by selecting the All nets check box in the Crosstalk Setup dialog box.

4.	Set up Polaris by selecting Polaris Setup.  Specify layout and board stack files.  If necessary, configure Polaris further by setting its extraction parameters in Crosstalk setup.

The fields in the dialog indicate which of these steps have been performed.  If a required step has not been completed (for example, if no .asc file exists, indicating that the layout has not been created), then the dialog fields for the subsequent steps would be shaded, indicating that they are disabled.

Invoke Polaris to extract transmission line information from the specified PCB layout file by clicking on the Extract button.  Polaris will use the parameters defined in the Polaris Setup and Crosstalk setup dialogs.  Extraction will be performed only if:

1.	the extraction parameters have been set up

2.	the PCB netlist file used as input to the layout editor exists

3.	the specified board stack file exists

4.	the specified PCB layout file exists

If any of these conditions are not satisfied, the Extract button will be shaded, indicating that it is disabled.

After parasitics have been extracted from the layout, you can view characteristics of the nets by clicking on the Select signals button.  In the list displayed, you can select whether or not nets should be included in the simulation.

The Select Signals button invokes the Select Signals dialog.  This dialog contains a listbox which shows the names of all nets for which parasitics have been extracted.

In addition to the name, the listbox shows the coupling factor (see the Signal Integrity manual) for this net, the length of the net, its total inductance, resistance, and capacitance, and the total amount of via capacitance connected to the net.  The list is sorted by coupling factor, so those nets most susceptible to crosstalk will tend to appear at the top of the list.

You can control which of the displayed nets are incorporated into the simulation with parasitics.  You can add nets either individually or by group.  Click on the Select Singly or Select Coupled buttons to select the appropriate mode, then select the entry[ies] in the listbox.

In Select Coupled mode, selecting a net adds the net plus any other nets which are mutually coupled.

The Clear button deselects all selections in the listbox.

Once the set of nets to include has been defined, you can simulate by clicking on the Simulate w/Parasitics button.  Note that if you selected All nets mode in Crosstalk setup, you MUST choose one or more signals through the Select signals dialog box after successful extraction for parasitics to be included in the simulation.

The Simulate w/ Parasitics button causes a PSpice simulation of the circuit to be run using parasitic data obtained from the extracted layout.  If the layout has not been successfully extracted, or if no PSpice analyses have been set up, then the button will be shaded, indicating that it is disabled.  The

Simulate w/o Parasitics button causes a PSpice simulation of the circuit as shown in the schematic to be run.  If no PSpice analyses have been previously set up, then the button will be shaded, indicating that it is disabled.  These two options allow you to examine the pre and postlayout behavior of the design.

The Auto check boxes on Simulate w/ Parasitics and Simulate w/o Parasitics will automatically queue up simulations to be run after the extraction has completed successfully.  They will not be available if All nets mode was selected in Crosstalk setup, since you will need to choose signals for simulation.

IMPORTANT:

If you enable automatic simulation after extraction, you must make sure that you are editing the schematic whose layout was extracted when the extraction completes.  Otherwise, you will be asked to reload it.  A negative response will cancel the simulation(s).

See Also

Polaris Setup

Crosstalk Setup


Polaris Setup

Minimum transmission line length specifies a threshold value for the line length below which the transmission line effects should be considered irrelevant for the operating frequency(ies) of the design.

The Routed PCB file field displays the name of the PCB layout file selected using the Browse PCB files button.  Similarly, the Board Stack field displays the name of the board stack file selected using the Browse board stacks button.

The Create board stack button will cause a file whose name is specified in the Board Stack field to be opened in a text editor window.  The text editor to be used is specified in the EDITOR entry in the MICROSIM section of your msim.ini file.  Refer to Board Stack File Format in the Signal Integrity Option manual for a discussion of the board stack file format.

The Crosstalk setup button invokes a dialog allowing you to set up crosstalk parameters and signal selection modes for the extractor.

The View signals button displays the list of device pin numbers or named nets for the signals to be extracted.  Each signal is specified by attaching a Polaris marker to one of the signal device pins or named nets in the schematic.  To change the list of signals to extract, Polaris markers must be either added to or deleted from the schematic.

See Also

Polaris

Crosstalk Setup


Crosstalk Setup

The Crosstalk setup dialog contains fields for setting the constraints used by Polaris during extraction and crosstalk calculations.

Crosstalk Mode instructs Polaris to operate in one of the following modes

Marked, coupled nets: extract each specified signal separately and find the lines that are coupled to it (Victim)

Marked nets only: extract the specified signals and determine the coupling between them (List)

All nets: extract all signals present in the routed PCB file (List)

Maximum number of Neighbors specifies the maximum number of neighboring conductors (on any layers) for which Polaris will retain coupling information.  If the number of conductors coupled to a particular line exceeds this maximum, Polaris will include only the most strongly coupled lines in the output file.  To determine which lines are more strongly coupled, Polaris compares the backward crosstalk coefficients of the coupled lines.

Maximum Search Radius defines the extent to which Polaris will search about a given conductor for a coupled conductor.

Minimum Parallel Run Length specifies the threshold distance beyond which two lines must extend in parallel before they will be considered coupled.

See Also

Polaris

Polaris Setup


Adding a DSL Block

A DSL block is a hierarchical block which contains a textual definition.  Each DSL block is associated with a DSL PROCEDURE in a DSL source file.  Each pin on the block corresponds to one of the procedure's input or output nodes.  The name of the DSL procedure is specified in the block's PLMODEL attribute.

To Add a DSL Block:

1.	Use the Draw/Block command and place the block on the schematic page.  You can resize the block by positioning the pointer near a corner of the block and dragging the mouse while pressing SHIFT and holding down the right mouse button.

2.	Add pins to the block by connecting wires or buses directly to the block.  Pins on the left side are automatically designated as inputs and pins on the right are designated as outputs.  You can change a pin's name or direction by double-clicking on the pin name to bring up the Change Pin dialog.  The pin's direction is specified in the ERC field.  (DON'T CARE is not allowed on DSL blocks.)  If a bus is connected to the block, the pin name must use the Schematics bus label format, e.g. ADDR[7-0].

NOTE: Pin names must be valid DSL identifiers.

3.	Push into the block by double-clicking on it, or by selecting Navigate/Push.  Because the block is new, the Setup Block dialog will appear.  Enter the name of the DSL source file you want to create or reference, then press OK.  You must use the .dsl extension to create a DSL block.  The DSL file will be loaded in the DSL Model Editor.

NOTE: The .dsl file name must not start with a digit (0-9).  In addition, it may not have the same base name as the schematic file.  It is reserved for system use.

For new DSL procedures, Schematics automatically creates a procedure template with input and output nodes corresponding to the DSL block's pin names and directions.  If no PLMODEL attribute is specified on the block, Schematics will use the DSL file name (less the .dsl extension).  Schematics also translates the bus label format to DSL array format.

Attaching a DSL Block to an Existing Procedure

1.	Place a block using the method described above.  Pin names must match the procedure interface node names in the DSL procedure.

2.	Use Edit/Attributes to add a PLMODEL attribute, specifying the DSL procedure's name as its value.

3.	Push into the block, and enter the name of the existing DSL source file in the Setup Block dialog.

Changing the DSL Block

The pins on the DSL block must match the port nodes of the DSL procedure, in number, name, and direction.  Thus, if you add or delete pins, or change the width of a bus on your DSL block, you must make sure that you update the procedure's port nodes corresponding to the changed pins.  If you change a port's direction (e.g. from an output to an input) you must change the ERC value of the corresponding DSL block pin.  To do this, you can double-click on the DSL block pin or use the Edit Pin ERCs button in the DSL Model Editor.

See Also

DSL Language Reference

Using the DSL Model Editor


DSL Model Editor
Using the DSL Model Editor

The DSL Model Editor allows you to edit DSL source files from within Schematics.  The editor is invoked by selecting a DSL block and using Navigate/Push or double clicking on the block.  When the editor starts, the selected DSL block's procedure will be positioned in the editor window, and the block's procedure name will be displayed in the Procedure Name field at the top.

Editing DSL Source

The editor follows the Microsoft Windows default dialog and edit field conventions.  The following accelerator keys may be used.

Key	Action

CTRLX	Cut

CTRLC	Copy

CTRLV	Paste

CTRLZ	Undo/Redo

CTRLTAB	Tab

The TAB key by itself will move focus to the next field in the dialog.

Checking Syntax

To perform a syntax check, press the Check Syntax button.  The current file will be saved in a temporary file, and PLSyn will be invoked to perform the syntax check.  If there are errors, a warning message will appear and you will have the opportunity to view the compiler log file.  If there are no errors, a Syntax check successful message will appear in the Schematics status line.

Changing Pin Directions on the DSL Block

If you need to change the direction of any pin on the DSL block, you can do so from within the DSL Model Editor by pressing the Edit Pin ERCs button.  This brings up a dialog containing the list of block pin names and their current ERC values.

Saving Changes

To exit the DSL Model Editor and save changes to the source file, press OK.  Schematics will check to make sure that each DSL procedure interface node corresponds to a DSL block pin, and vice versa.  A warning message will appear if there are any differences.

Aborting Changes

To exit the DSL Model Editor without saving changes to the source file, press CANCEL.

See Also

DSL Language Reference

Adding DSL Blocks


Importing OrCAD Schematics

Schematics can translate schematics created with OrCAD into Schematics format.  Once they are translated, you can then edit them with Schematics.

Note that this is a one way process.  Any changes you make to the schematic or symbol library with Schematics cannot be read by OrCAD.

When translating OrCAD schematics, Schematics uses the OrCAD configuration file, sdt.cfg, to determine which OrCAD symbol libraries to use to find symbols.  Symbols referenced by the schematic are translated and put in a Schematics local symbol library.  The sdt.cfg file must be either in the same directory as the OrCAD schematic or in the TEMPLATE subdirectory under the directory pointed to by the environment variable ORCADPROJ.

Although Schematics makes every attempt to translate the schematic completely, there may be discrepancies in the resulting schematic depending on how certain features of OrCAD were used.  You should always check any errors and warnings that occur during the translation as well as reviewing the resulting schematic.  See Tips on Translating OrCAD Schematics for further details.

Translating Multi-Page Schematics

To translate a multi-page schematic, translate the root page (the page containing the ILINK text that lists the files of the other pages).  All pages referenced by the ILINK text will be translated.  Schematics keeps all pages of a multi-page schematic in a single file so there will only be one resulting schematic file, the root, which contains all the pages.

Translating Hierarchical Schematics

To translate a hierarchical schematic, translate the topmost sheet.  Any subschematic referenced by sheet symbols will also be translated.

See Also:

Import Command (File Menu)


Tips on Importing OrCAD Schematics

Text Size

.	Text sizes on translated schematics/symbols are based on an 8 point font size.  You can use the Editor Configuration command in the Options menu to change the font that Schematics uses for text display.

Differences between OrCAD and MicroSim Schematics affecting translation

1.	In OrCAD, you can have ports with multiple connections.  This is translated as two ports overlaid with pins facing opposite directions.

2.	Schematics has fixed size ports.  I.e. they do not resize based on the label.  When an OrCAD schematic is translated  port symbols are created for each port size.

3.	In Schematics, wires connect directly to buses without using special symbols such as bus entries.  Buses MUST be labeled with the set of signals they represent.  Wires connected to buses must be labeled with the signal name within the bus to which they correspond.

Therefore, during translation,

.	OrCAD "Bus Entry" objects are converted into regular wires.

.	 When drawing "bus rippers" users must use the OrCAD "Bus Entry" object and not
simply draw a normal wire at an angle to look like the regular bus ripper/entry object.
Otherwise the wire is not connected to the bus.

4.	Dashed annotation lines are not included in the translated schematic.

5.	Text with an orientation of:

T
h
I
s

is translated into rotated text.

6.	De-Morgan equivalents (convert symbols) are not supported.  You get the non-converted version on your schematic.

7.	The 'Simulation' attributes that are added to symbols are based on the OrCAD standard libraries. Therefore pin name references in these attributes are could potentially be incorrect if a different (as in user drawn) part is being used by the same name.

8.	Wires that cross pins exactly at the pin hotspot will be connected.

9.	Unlabeled wires connected to buses will not be connected to the bus.

10.	The OrCAD feature of pins with number zero not being drawn is not supported. Therefore some symbols are drawn with unexpected pins or with missing pins. Only the first (GATE A) representation of the symbol is translated.

11.	Fill patterns used in parts are not translated.

12.	No Connect symbols on the OrCAD schematic are not translated (nor are Stimulus, Trace or Layout symbols)

Translating Large Designs

A standalone version of the translator, orctrans.exe is provided for translating large designs.


Help Topic Title Style (Non Scrolling)

Syntax	this is the syntax definition line 1
this is the syntax definition line 2

Parameter List Title	Description

Parameter List Style	Parameter list is intended to follow a syntax definition because it allows for keywords using a hanging indent.

Normal Style

Subsection

Normal

1.	List style, line 1

2.	List style, line 2

Menu Style	Description of menu command.  Includes a hanging indent like parameter list.

Example Style

Example Text Line 1
Example Text Line 2


New Command (File Menu)

Creates a new schematic.


Open Command (File Menu)

Opens an existing schematic for editing.  You may enter the file name of a schematic, or choose from the list of schematics that appear.  You may also modify the path in order to select schematics in other directories by entering the path name, or by clicking on an entry in the list of directories.


Save Command (File Menu)

Writes the current active schematic to a file.  If the schematic is new, the Save As dialog will appear allowing you to type in the new schematic file name.  If a schematic with this name exists, the previous version is first copied to your backup directory and the current schematic is saved.  Any changes made to any of the pages in any window are saved.


Save As Command (File Menu)

Saves the currently active schematic to another file name.  Unless otherwise specified, the schematic is automatically saved into the current working directory.  If you wish to save it to a different directory, enter or select the path name of the directory you wish to save it to


Close Command (File Menu)

Closes the currently active schematic  All windows showing any page of the schematic are closed.  If the file has not been saved, you will be prompted to save the changes before the window is closed.


Import Command (File Menu)

Loads a schematic created with OrCAD into Schematics for editing.  The schematic and any symbols it uses are translated from OrCAD's format into Schematics' format.  This is a one-way process.  You may also translate individual OrCAD libraries with this command.

Dialog Box Options

Input File
Name of the OrCAD schematic or library to be translated.

Destination Directory
Directory where the translated schematic is to be created.  The translated schematic will have the same name as the original OrCAD schematic.  A translated symbol library will have the same name but have the extension .slb.

Options

Include Simulation Information
Causes simulation attributes to be added to symbols in the library as well as converting part field information on the schematic into information that can be used by the Schematics simulation netlister.  The attributes in the part field conversion is based on mapping files devmap.ini and orc_map.txt.  These contain default information based on the standard OrCAD libraries.  You can change or add additional parts to these files with any text editor.

This option should be enabled if you plan to simulate your designs using MicroSim PSpice or MicroSim PLogic. If enabled, the PSpice Simulation Device Types Dialog, described below, will be displayed.

Include PCB Information
Creates package libraries in addition to symbol libraries during translation.

This option should be enabled if you plan to netlist the schematic for layout.  If enabled, the Package Types Dialog, described below, will be displayed.

Package Types Dialog Options

To assign package types (footprints) and create package definitions for the parts on your schematic, Schematics uses the file orc_map.txt to search for default package types.  A list is created of all parts for which no entry was found.  The Package Types dialog lets you assign package types for these parts.  The default is to make the package type (footprint) name the same as the part name.

Part
List of parts for which no default package information was available.

Package Type
List of current package types to be assigned to the corresponding parts.  The initial default is to assign a footprint with the same name as the part.

Package Types
Name of the package type to assign to the currently selected part(s).  You can enter a name or choose one from the list.

Set Package Type
Assigns the package type in the Package Types field to the currently selected part(s).

PSpice Simulation Device Types Dialog Options

To convert OrCAD part field information need for simulation, Schematics must know the PSpice device type for each part placed on the schematic.  An initial guess is made during translation, based on the first letter of the reference designator.  The PSpice Simulation Device Types dialog displays the list of parts and the translators initial assignment of device type.  You use this dialog to review the list and make any necessary corrections.

The conversion of part field information is converted by the mapping file, devmap.ini file.  For each PSpice device type, the map file lists the OrCAD part field corresponding to the simulation device parameter(s) for that device type.  Devmap.ini is a text file which you may need to modify depending on how you used OrCAD part fields.

Part/Refdes
List of each parts symbol name and reference designator on the schematic.

Device Type
List of current PSpice device types to be assigned to the corresponding parts.

Available Device Types
A complete list of PSpice simulation device types.

Set Device Type
Assigns the device type in the Available Device Type field to the currently selected part(s).

See Also:

Importing OrCAD Schematics

Tips on Importing OrCAD Schematics


Print Command (File Menu)

Prints one or more pages of the current schematic.   In the dialog, select the desired page(s) to print from the list that appears by clicking on a selection.  Choose Select All to select all of the pages of the current schematic.

Dialog Box Options:

Current Printer
Shows the current default printer.  The printer can be changed through the Printer Select button (see below) or through the File/Printer Select command.

Scaling options
Controls the size of the printout:

Auto-fit
Scales the size of the page to print one schematic page per sheet of printer paper.  For example, if the schematic page, (set through the Page Size command in the Options menu), is B-size and your printer paper is A-size, Auto-fit automatically sets a zoom factor of 50% so that the B-size drawing fits on the A-size paper as shown in

User-definable zoom factor
Sets a custom zoom factor.  For example, with the zoom factor set at 100%, a B-size schematic will print on two A-size sheets of paper when the printer is configured in portrait mode.

With the zoom factor set to 200%, a B-size drawing will print on eight sheets of paper.  Doubling the zoom factor quadruples the number of printer pages needed to print a schematic.

With User-definable zoom enabled, the printer configured in portrait mode, and a 100% zoom factor,.

·	An A-size schematic will print on two sheets of A-size paper

·	A B-size schematic will print on two sheets of A-size paper

In landscape mode, using a 100% zoom factor:

·	An A-size schematic will print on one sheet of A-size paper

·	A  B-size drawing will print on four sheets of A-size paper

Orientation
Controls the output orientation of the print. Since schematic pages are wider than they are high, if you want the schematic to appear as large as possible on the printed page, the printer should be configured in landscape mode.

Auto-Fit will work in portrait mode, but the schematic will be printed in the upper portion of the page.

Page Setup
Invokes the Page Setup dialog for setting the margins for the printed page.  Margin defaults are 1/2" or 15mm.  Setting up different margins modifies the area the schematic page will occupy if Auto-fit is selected.  If User-definable zoom factor is selected, the drawing will be the specified size, but offset by the margin values.

Printer Setup
Displays the setup options for the currently selected printer.  This dialog will vary depending on the printer that you are using.

Printer Select
Selects of another printer to use for printing the schematic.  This displays the same Printer Select dialog as the File/Printer Select command (see below).

Only Print Selected Area
Prints the only portion of the schematic currently selected when the File/Print command is issued.  To select the print area place the cursor at one corner of the area, press and hold the left mouse button, and drag the cursor to form the bounding rectangle.


Printer Select Command (File Menu)

Select a printer to use with Schematics and sets up printing options. Once you have selected a printer from the list, use the Setup command to display the configuration options for your particular printer.  Your printer configuration for Schematics will stay the same until it is modified again through the Setup command.  The Schematics printer configuration is independent of other applications' printer configurations.  Set up the printer the way you wish, and click OK when you are finished, to copy the printer setup to "msim.ini."  Schematics will use the printer setup in "msim.ini" to configure the printer each time you print from Schematics.


Edit Library Command (File Menu)

Brings up the symbol editor window.  With this command, you can create new parts or edit existing parts in any of the library files.


Symbolize Command (File Menu)

Converts the current schematic into a symbol.  A symbol is generated (or updated) from the current schematic, and if new, you are prompted for a library file in which to save the symbol.

Interface ports must be placed on the schematic and given labels to provide external inputs and outputs to the symbol.  Pins are automatically created for the symbol with the names of these interface ports.  The shape of the symbol is rectangular, with its size calculated by the number and placement of pins.  Input pins are generated from IF_IN ports and placed on the left, output pins are generated from IF_OUT ports and placed on the right, and other pins are generated from the generic INTERFACE port and placed where they fit best (left or right).

A hidden pin is added to the symbol for each global port or node referenced in the schematic.  The hidden pin name will be the same as the global port name.  Hidden pins are placed on the top or bottom of the symbol. As with all other hidden pins, an IPIN(<pinname>)=  attribute will be added to the symbol attribute list for each hidden pin, and each will have the port name as its value.


Reports Command (File Menu)

Generates a bill-of-materials report for the current schematic.  Each entry includes component type (part number), the quantity of each type, and respective reference designators for each component in the schematic.  You can customize the report to include additional attribute information by using the Reports Setup dialog (described below).  This additional information can be from information on the schematic or from a user generated component description file that can be generated from an external database.

Dialog Box Options

Display
Sends the bill-of-materials report to the screen.

Print
Sends the bill-of-materials report to the currently selected printer device.

Setup
Displays the Reports Setup dialog which lets you specify a list of attributes and descriptive text to be included in the bill-of-materials report for each component type.

Component Description File
Name of the component description file (".cdf") to be used.  This is a file of additional in-house information on parts such cost, internal part numbers, suppliers, etc. and is in a standard database format so that it can be easily generated from in-house databases.  An example file, user.cdf, is shipped with Schematics.

Format
Specifies the attributes to be displayed in the report.  Each attribute is specified using the syntax

      [descriptive text]@<attribute name>

where the `@' sign indicates value substitution for the named attribute.  Multiple attributes are specified using the above syntax in a comma-separated list.  For example, you could specify that the part instance VALUE attribute, and your own user-defined attributes-COST and ADDR-be reported by entering the following into the Format text box:

     value = @VALUE, cost = @COST, address = @ADDR

Print Output Format Parameters:

Text, when selected, formats the bill-of-materials list in ASCII format with one entry per component type.

Database, when selected, formats the bill-of-materials list with one attribute name/value pair per entry; thus, there will be multiple entries for component types with multiple attributes.

Save As
Writes the bill-of-materials report to a file.  A standard Save As dialog is displayed.


Current Errors Command (File Menu)

Displayed the list of current errors.  The errors are displayed in a scrollable window box that appears when you choose this item.

Dialog Box Options

Goto
(If there is an X, Y value associated with the currently selected error), scrolls the viewing area so that the X, Y is centered in the middle of the viewing area, and positions the cursor at that location.

Print
Prints the error list to a file or a printer device.

Clear
Deletes all errors from the list.


Exit Command (File Menu)

Exits MicroSim Schematics.  Schematics will prompt you to save unsaved changes in a schematic or symbol library.


Undelete Command (Edit Menu)

Restores the item(s) last Cut (deleted) from the schematic.  Undelete returns the item(s) in the buffer to the exact position on the schematic where it was deleted and clears the buffer.


Cut Command (Edit Menu)

Deletes selected item(s) from the schematic and copies them to a buffer for use with the Paste command.  The Cut command retains only the last item (or set of items) in the buffer.

See Also:

Selecting Items on a Page


Copy Command (Edit Menu)

Makes a copy of the selected item(s) for later pasting.  Select the item(s) on your schematic to be copied.  After choosing Copy from the menu, choose Paste to place the copied item(s) onto your schematic.

See Also:

Selecting Items on a Page


Paste Command (Edit Menu)

Paste places one or more copies of the last item(s) stored in the buffer (from the Cut or Copy command) onto the schematic.  When you choose Paste, the cursor takes on the shape of the object(s) last copied or deleted.  Click to place the item(s) at the current cursor location.


Copy to Clipboard Command (Edit Menu)

Copies an image of a selected rectangular area on the schematic to the Microsoft Windows Clipboard for use in other Windows programs.  No electrical or connectivity information is copied to the clipboard.  For example, you might want to make a copy of your schematic to include in another type of file, such as a word processor file.  You must first select a region to be copied, then invoke the Copy to Clipboard command.

See Also:

Selecting Items on a Page


Delete Command(Edit Menu)

Delete deletes the selected item(s) from the current schematic.  The paste buffer is not affected.


Edit Attributes command (Edit Menu)
Attributes Command (Edit Menu)

Attributes allows you to edit the attributes of a currently selected object(s).  If an object such as a part is selected, the Edit Attributes dialog is displayed.

Note:  Any changes you make to the part attributes are made to individual part instances.  The original part contained in the library file remains unchanged.

Attributes preceded with an asterisk (`*') cannot be modified directly from this dialog, but must be changed through the Symbol Editor.  An `a' indicates that the attribute has been annotated as a result of back annotation or has been assigned by the packager.

You can also bring up the dialog by double-clicking on a selected part.  This method saves you the step of opening the Edit menu.

To change an attribute:

Select an attribute name/value pair from the list box.  The name and the value of the attribute will be displayed in the corresponding edit controls.  To change an attribute name, type in a new name in the Name text box, and click Save Attr.  To change an attribute value, type in a new value in the Value text box, and click Save Attr.  The changes will be immediately reflected in the list box. Click on OK to save the changes.

To add a new attribute

Type in an attribute name in the Name text box, then type in a value in the Value text box.  Click Save Attr to add the name/value pair to the attributes list box.  Click on OK to save the new attribute(s).

To delete an attribute

Select the name/value pair, and ensure that they appear in the corresponding edit controls.  Click Delete to remove them from the list.  Click OK to confirm the deletions.

Dialog Box Options

Include Non-changeable Attributes
Controls display of attributes that are not changeable from within this dialog.

Include System-defined Attributes
Controls display of attributes that are defined automatically by Schematics.

Change Display
Displays the Change Attribute dialog.  This dialog lets you specify whether the attribute name, value, or both will be displayed on the schematic.

Changeable in Schematic when enabled, allows the attribute value to be edited in the Schematic Editor.

Display Value when enabled, specifies the attribute value to be visible on the schematic.

Display Layer defines the layer upon which the attribute name and/or value will be displayed.  Whether a layer is displayed and/or printed can be configured using the Options/Set Display Level command.

Display Name when enabled, specifies that the name of the attribute will be visible on the schematic.

Size defines the size of the text as a percentage of the default text size (defined in msim.ini)

Orientation defines the rotation of the text.

Hjust defines the horizontal justification.

Vjust defines the vertical justification.


Label Command (Edit Menu)

Label places a label on selected wires, bus segments, or ports.  Wire and bus segments may display multiple labels; however, all labels for a wire or bus will contain the same text.

To edit a label, select the label, and choose Attributes, or double-click on the label itself.

See Also:

Labeling Wires, Buses and Ports


Model Command (Edit Menu)

Lets you to edit the simulation .MODEL or .SUBCKT definition for a part.  Edit/Model is designed to make an individual copy of a model or subcircuit representation, allowing you to modify the copy.  These changes will only apply to the specific part instance in the  current schematic.  By default these individual instance models are saved in a file with the same name as the originating schematic file, and a ".lib" suffix.

You can change the model used in that instance of the part through either the Model Editor dialog or through the Parts program.

To edit a model, select a part, then select Edit/Model.  This will bring up the Edit Model dialog if the part instance has a MODEL attribute.  The Edit Model dialog will give you the choice of changing the name of the model referenced by the selected part, or editing an instance model (a copy) of the part.

Dialog Box Options

Change Model Reference
Brings up a dialog that allows you to enter the name of another model for this part instance.  Enter the new model name and click on OK to accept.

Edit Instance Model (Text)
Displays the model editor dialog which lets you edit a copy of the model or subcircuit definition.  If an instance model does not already exist, the Schematic Editor creates a new instance model definition that is a copy of the original model.  The Schematic Editor will append a -X, -X1, -X2, etc. to the model name to distinguish it from the base model name.  If an instance model already exists, it will be copied for editing.

Note that you must use the text-based model editor to edit any model type which is not supported by the Parts program, and to add Monte Carlo parameters.

Expand AKO
Searches through any AKOs the model might have and add these new parameters to the model.  This command essentially flattens a hierarchy of AKOs into one model definition where you can see all the parameters.

Edit Instance Model (Parts)
Invokes the Parts program for editing of the model definition.  This option may be used to edit models which are supported by the Parts program.  (Refer to the Circuit Analysis User's Guide for information on the Parts program for Windows.)

Note:  The Schematic Editor will not allow you to edit the underlying base model or subcircuit definition of the symbol; this must be done from the Symbol Editor.


Stimulus Command (Edit Menu)

Invokes the Stimulus Editor. If you have not selected a stimulus symbol, the Edit Stimulus dialog will be displayed.  This dialog allows you to edit all stimulus on the current page, on any page of the current schematic, or all stimulus symbols in a hierarchical design.


Symbol Command (Edit Menu)

Opens the Symbol Editor window with the symbol of the currently selected part loaded.  When the Symbol Editor window is active, the menu bar at the top of the main window reflects the commands for the Symbol Editor.


Views Command (Edit Menu)

Displays the Edit Views dialog which lets you to display, add, or change the schematics associated with a selected block or hierarchical part.   First select the part or block then select the Edit/Views command.  The views and associated schematics are listed in the dialog.

For hierarchical blocks, the list of views can be edited in this dialog.

For hierarchical parts, changes must be made through the Symbol Editor's Edit/Set Schematic command.


Convert Block Command (Edit Menu)

Converts selected block(s) in the active window to symbol(s), checking for consistency of represented schematics with block information.


Rotate Command (Edit Menu)

Rotates a selected object(s) 90 degrees counterclockwise.  If you select an area of your schematic, the area is rotated around the center of the selection box.


Flip Command (Edit Menu)

Flips a selected object(s) to produce a mirror-image of the object.


Align Vertical Command (Edit Menu)

Moves all selected objects (symbols, wires, text, etc.) so that their origins are along the same vertical line.  Objects are aligned with the leftmost object.


Align Horizontal Command (Edit Menu)

Moves all selected objects (symbols, wires, text, etc.) so that their origins are along the same horizontal line.  Objects are aligned with the topmost object.


Replace Command (Edit Menu)

Replaces parts on a schematic with a different part.

Dialog Box Options

Target Part
Name of the part you want to be replaced.

Replacement
Name of the part you want to replace the old part (target part) with.

Keep Attribute Values
If enabled, keeps the target part's attribute values, instead of being overwritten by the replacement part.

Selected Parts Only
If enabled, replaces only parts that are currently selected.  If enabled, no Target Part name is required.

Current Page Only
If enabled, all target parts on the current schematic page in the active document window will be replaced.

All Pages
If enabled, all instances of the target part on all pages of the active schematic will be replaced.


Find Command (Edit Menu)

Searches for parts, wires, and buses on a schematic based on given search criteria.  The Find command allows you to enter one or more attribute name/value pairs as criteria.  Parts, wires, and buses which contain attributes whose values match the search criteria are then selected on the schematic.

Dialog Box Options

Name
Attribute name to match.

Value
Attribute value to match.  You may specify an exact value or use wildcards to specify a search pattern.  An `*' will match zero or more characters.  For example, R* will match both R1 and R12.  A `?' indicates a wildcard, and will match any single character.  For example, R? will match R1, but not R12.

Note:  Searching is case insensitive.

Clear current selection
Specifies that all currently selected items will be deselected prior to the search.

Select All
Specifies that all items meeting the search criteria will be selected.

Select Next
Specifies that only the next item meeting the search criteria will be selected.  The first time new criteria are entered, Find will select the first item it finds meeting the given criteria.  Subsequent searches with the same criteria will find the next item meeting the search.  When the last item is found, a message will appear reporting End of Search.  Searching again with the same criteria will again find and select the first item.

Using the Draw/Repeat command after a search with Select Next chosen, is a quick way of finding the next item.

Add Criterion
Lets you specify more than one search criterion.  Only items meeting all criteria will be selected.

Delete All Criteria
Clears all current search criteria so that new criteria may be entered.

OK
Starts the search.  The number of items found and selected will appear in the status bar at the bottom of the Schematics window.  The cursor will be moved to point at the first item.


Repeat Command (Draw Menu)

Repeats the last menu command used in the currently active window.  If you have the  same schematic displayed in multiple windows, each window retains a different repeat command.  The result of each command will be reflected in each of the windows for that schematic.  The command currently in the repeat buffer is displayed in the status line of the main window.


Place Part command (Draw Menu);parts, placing
Place Part Command (Draw Menu)

Places an instance of the current part onto the schematic page.  The current part is the part last specified by the Get New Part command for that document window.

After selecting Place Part, the cursor is replaced by the shape of the part.  You may rotate or flip the part before it is placed by using <Ctrl R> (to rotate), or <Ctrl F> (to flip).  Each click places an instance of the current part.

Double-click to place the part and end the function, or click right to end without placing the part.  The last placed part remains selected so that you can operate on it further if required.

If Auto-Naming is enabled, a unique reference designator is automatically assigned to a part when it is placed.


Text Command (Draw Menu)

Places text on the schematic.  You may place text anywhere on the current schematic page.  In the dialog, type in the desired text and select OK.  Then, move the text to the desired location on the schematic, and click to place the text.

To change the text size, select Size and modify the default size (100%) to suit your application.  (Windows users can also change the size and font for all text on a schematic using the Options/Editor Configuration/Fonts command and selecting an available font.


Wire command (Draw Menu);wiring
Wire Command (Draw Menu)

Draws wires consisting of one or more segments.

When you choose Wire, the cursor changes to a pencil shape.  On your schematic, place the cursor at the point where you want the wire to start.  Click to anchor the wire and begin drawing.  Move the mouse in any direction to extend the wire.  You can now either double-click to end the wire and terminate the mode, or continue moving the mouse and clicking to draw more wires.  Ending a segment on a pin or the middle of another wire or bus segment will terminate the wire but leave you in wire mode, ready to start a new wire.

Use the Snap to Grid feature and the Orthogonal feature to facilitate drawing wires.

See Also:

Labeling Wires, Buses, and Ports

Display Options Command (Options Menu)


Bus Command (Draw Menu)

Draws busses consisting of one or more segments.

When you select Bus, the cursor changes to a pencil shape.  On your schematic, place the cursor at the point at which you want the bus to start.  Click to anchor the bus and begin drawing.  Move in any direction to extend the bus. Ending a segment on a pin or the middle of another wire or bus segment will terminate the wire but leave you in wire mode, ready to start a new bus.

See Also:

Labeling Wires, Buses, and Ports


Block Command (Draw Menu)

Places one or more hierarchical blocks on the schematic page.

To change the size of a block:

Once a block is placed, it may be stretched by selecting the block, placing the cursor on or inside any of its edges, and dragging the cursor with the <Shift> key and right mouse button depressed (on the PC).  As the cursor is dragged, an outline of the stretched block will appear.  Click and release when the block is the desired size.

To create pins on a block:

Wires and buses that end at any of the edges of the block will automatically connect to the block.  Pins will be created where the connections occur.  A default pin name will appear within the block.  You may edit a pin name by selecting the pin name, and choosing Attributes from the Edit menu.  Or you may simply double-click on the pin name to bring up the Edit/Pin dialog.  To delete a pin, select the pin and choose Delete from the Edit menu.

To associate an existing schematic with the block:

Use the Edit/Views command.

To create a schematic for the block,

Use the Navigate/Push command.


Get New Part Command (Draw Menu)

Displays the Add Part dialog which lets you select a part and/or browse the list of available symbols. If you know the name of the part, enter the name of the part in the Part text box, and press <Enter>.   (If you type a part name in with <Caps Lock> turned on, the part will be placed with all capital letters.)

Or, you can choose Browse to review the list of parts in the configured library files.  When you choose Browse, a dialog appears displaying a list of library files and the parts they contain.  Either double-click on a library part to bring up the part, or select the desired part and click OK.

Once a selected part has been retrieved from a Symbol Library, an outline of the part will appear allowing you to place one or more instances of the part anywhere on the schematic.

Before a part is placed, or while it is still selected, you can rotate (<Ctrl R>) or flip (<Ctrl F>) the part to the desired placement position.

Use <Ctrl G>, as a shortcut to bring up the Add Part dialog, or once a part has been placed, double-click right to place one or more instances of the same part.

This command also designates the chosen part name as the current part, which is the default for the Place Part command.  The current part name is displayed in the main menu bar.


Rewire Command (Draw Menu)

Reroutes a selected wire or bus segment without disconnecting its end points.  After choosing the Rewire command, select a point on the wire or bus segment to rewire.  As you move, the wire or bus segment stretches as indicated by the cursor.  Either click to set a vertex, or double-click to set the segment and end the rewiring mode.


Previous command (Navigate Menu)
Previous Page Command (Navigate Menu)

Displays the previous page of a multi-page schematic in the currently active window.


Next command (Navigate Menu)
Next Page Command (Navigate Menu)

Displays the page following the current page of a multi-page schematic in the currently active window.


Select Page Command (Navigate Menu)

Displays the list of pages for the currently active schematic and lets you select one to display in the currently active window.


Create Page Command (Navigate Menu)

Adds a new page to the current schematic.  You may specify a title (used in the Title Block) for the page.  The new page will be added after the current page, and will be ready for editing.  To change the page title, choose Edit Page Info (see below).


Delete Page Command (Navigate Menu)

Deletes the current schematic page.  You will be requested to confirm the deletion.


Copy Page Command (Navigate Menu)

Copies one or more pages from either the current schematic, or another schematic, into the current schematic.  The copied page(s) will be inserted after the current page, and all pages will be renumbered.  In the dialog, specify the name of the schematic you want to copy from, the directory in which it is found, and the page number(s) to copy.


Edit Page Info Command (Navigate Menu)

Changes the title of the currently active schematic page.

Dialog Box Options

Simulation Only
If enabled, indicates that the entire page is to be ignored for purposes other than simulation.


Edit Schematic Instance Command (Navigate Menu)

When enabled, displays instance specific attributes associated with the instance of the block or hierarchical symbol into which you are pushed.  While in this mode, you can only delete and change annotated attributes.  These changes will only apply to this instance of the hierarchical block or symbol into which you are pushed.  To make changes to the schematic itself, use Navigate/Edit Schematic Definition.

This command is available only if you have pushed into a subschematic.


Edit Schematic Definition command (Navigate Menu)
Edit Schematic Definition (Navigate Menu)

If enabled, displays the underlying schematic into which you are pushed with no instance specific information (such as reference designators).  Changes made will affect all instances of hierarchical blocks and symbols that reference this schematic.


Push Command (Navigate Menu)

Displays the subschematic represented by the selected hierarchical symbol or block in a new window.

If the selected symbol represents more than one schematic (has multiple views), a dialog is displayed allowing you to choose which schematic to edit.  Push allows you to push into a selected hierarchical symbol or block and edit its underlying schematic.


Pop Command (Navigate Menu)

Closes the currently active window that is displaying a subschematic and  displays the schematic up one level hierarchy.  If any changes have been made to the current level in the hierarchy, the user is prompted to save the modifications or to move up to the next higher level without saving changes.


Top Command (Navigate Menu)

Closes all subschematics of the currently active design and displays the window showing the topmost schematic.


Where Command (Navigate Menu)

Shows the hierarchical path of the currently active schematic.  This command brings up a dialog informing the user where this schematic fits in the hierarchy of the current design.


Fit Command (View Menu)

Sets the viewing scale to show all parts (excluding the title block),  wires, and connectors within the viewing window.

The actual fit percent (that is, the measure of how closely the window fits the contents) is configurable through the Pan & Zoom command in the Options menu.


In Command (View Menu)

Changes the viewing scale so that you to view your schematic at a closer range, so that items appear larger.  Use the cross hair to select the center of the viewing area.

The amount that the viewing scale is changed is configurable via the Pan & Zoom command in the Options menu.


Out Command (View Menu)

Changes the viewing scale so that you can see a larger area of your schematic.  Use the cross hair to select the center of the viewing area.

The amount that the viewing scale is changed is configurable via the Pan & Zoom command in the Options menu.


Area Command (View Menu)

Displays the selected area on the current schematic at the optimum viewing scale so the area fills the screen.  If an area is already selected it will be used; otherwise define the area by clicking and dragging.


Previous Command (View Menu)

Change the zoom factor and viewing area back to what it was previously.


Entire Page Command (View Menu)

Displays the entire schematic page at once.


Redraw Command (View Menu)

Redraws (refreshes) your screen display.


Pan New Center command (View Menu)
Pan - New Center Command (View Menu)

Retains the current zoom scale and pans the schematic so that the point selected is centered in the display.


Display Options Command (Options Menu)

Customizes various features of the screen display.

The options in the Display Options  dialog will be applied to all schematic windows and are explained below.

Dialog Box Options

Grid On
Turns the grid display on or off.

Snap to Grid
(Only applicable if Stay on Grid is enabled)
Causes components to snap to the nearest grid point when you place them; before placing, objects may be moved freely. If Snap to Grid is disabled, movement is by grid units as the mouse is moved (the cursor will jump to the nearest grid as you move the mouse).

Orthogonal
Constrains wire and bus segments to be horizontal or vertical lines.

Stay on Grid
Places components strictly on the grid.  Components always stay on the grid lines, even while being moved.

Snap to Pin
Causes the endpoint of a wire or bus segment to snap to the nearest pin if one is found inside the maximum radius; the radius value is that specified by the SnapToPinGravity variable in the [SCHEMATICS] section of "msim.ini." (see "Appendix A" in the Installation Manual).

Rubberband
Causes connectivity to be maintained when parts, ports, wires and buses are moved.  Additional wire or bus segments are added to accomplish this.

Status Line
Turns the status line at the bottom of your screen on or off.

Cursor X and Y
Turns the X and Y coordinates display (shown on the status line) on or off.  These coordinates are shown in inches if a US-standard page size is selected, or in millimeters if a metric page size is selected.

Toolbar
Turns on and off the displays the toolbar.

Grid Spacing
Defines the horizontal and vertical grid spacing on your drawing area.  The default spacing is 10 units.  This corresponds to (and is displayed as) .10 inches for US-standard page sizes, and 2.5 millimeters for metric page sizes.  The minimum grid spacing allowed is 0.01 (US sizes).

Text Grid
Sets the grid spacing for text separately from the normal grid spacing.  When Text Stay on Grid is enabled, this feature enables you to move text in very small increments along the lines of the grid.


Page Size Command (Options Menu)

Sets the page size for the currently active schematic page (i.e., the drawing size:  A-size, B-size, etc.).  This also becomes the default page sizes for any new pages that are created.

To set the page size,

Choose a page size from the list in the dialog and click in the box.  You may choose one of the standard page sizes (A, B, C, D, E, or A4-A0), or define your own dimensions.


Auto-Repeat Command (Options Menu)

When enabled, automatically places an object(s) identical to the previously placed object a specified distance apart.  The repeat function will then continue the action.  For example, you can use Auto-Repeat with the Place Part command to place repeated part instances, or with the Wire command to place multiple wire segments.

You can also use the <Space Bar> to repeat the previous command.  In the dialog, you can turn the following features on or off:

Dialog Box Options

Enable Auto-Repeat
Turns Auto-Repeat on or off.  Off is the default setting.  You can also use F8 and <SHIFT>F8 to turn on and off autorepeat.

Horizontal and Vertical Offset
Defines the distance in which objects are automatically placed in relation to the previous instance of the object.


Auto-Naming Command (Options Menu)

Dialog Box Options

Enable Auto-Naming
Turns the Auto-Naming feature on or off.  The default setting is ON.  When Auto-Naming is turned on, unique reference designators will be assigned as new parts are placed.

Starting Designator No.
Sets a number from which the automatic reference designator will begin numbering.  For example, if the starting number for an R device is 100, additional  R devices are automatically numbered R100, R101, R102, etc.  The default starting number is one.

Enable Auto-Increment
Turns the automatic increment feature on or off.  When enabled, Auto-Increment automatically increments the label specified under Label Template, below, for the port or wire selected, whenever the Label command is invoked.  Auto-Increment eliminates the need for the prompt requesting you to enter a label name.

Label Template
Provides the name that will be automatically assigned when Auto-Increment is on, and you place a label.  The label increments by one (i.e., using Auto-Increment, if the label is L101, the next one will automatically be labeled L102).  The default label name is the last label name used, incremented by one.


Set Display Level Command (Options Menu)

Turns off and on the display of certain categories of items and text for the screen and/or the printer.  The default is to display them both on the screen and on the hard copy.

Check boxes under Prt to specify items to appear on the hard copy.  Check boxes under Screen to specify items to appear on the screen.  Clear All will clear any choices that have been set.  Set All sets all choices to be displayed on the screen and to be printed on the hard copy.


Editor Configuration Command (Options Menu)

Sets various properties of the Schematic Editor, including Symbol Library files, library paths, page settings (such as the size of the drawing area), fonts, and configuration settings for other applications.

Dialog Box Options

Libraries
Provides a list of available library files used by Schematics when searching for a part.

Libraries that are prefixed by the `*' symbol are accessible by all schematics.  Otherwise, they are configured as local to the current schematic.

Library Path
Specifies the search path used by Schematics to find the library files in the library list.  Editing this text box modifies the path.  Schematics will first search the current working directory.  If the library file is not found, it will search each directory in the search path in the order specified.

Title Block Symbol
Specifies the title block symbol that is to be automatically added whenever a new schematic page is created.  You can create your own title block symbol in the Symbol Editor, and reference that symbol in this dialog.

Autosave interval
Specifies the time interval, in minutes, at which Schematics will save the current Schematic or library.  A time interval of 0 will disable autosaving.

When autosave is enabled, a temporary file is created with the same name as the current working file, and an extension ending in `v' (".scv," ".slv," ".plv," etc.).  If there is a power outage or system failure, you can retrieve your work from this file.  This file is deleted each time a schematic or library is successfully closed or saved.   When a file is loaded, Schematics compares that file to the autosave file, if one is present.  If the autosave file is more recent than the requested file, Schematics will provide a warning and allow you to restore it as the current schematic or library.

While an autosave is in progress, a message will appear in the status line and the hourglass cursor will appear.  Wait until the autosave is finished before continuing.

Monochrome Mode
Causes Schematics to operate in monochrome mode.  For example, selections are shown outlined rather than with a color change, independent of your monitor.

Library Settings
Displays the Library Settings dialog which lets you to add, modify, or delete the list of configured symbol and package libraries.

To configure a library that is available for all schematics:

Type a name in the Library Name text box.  When you indicate the type of file to be added (Symbol, Package, or both) by clicking in the box for the respective file type, this will add the default extension to the file name.  Click Add*. The library will be inserted above the currently selected library.

To configure a library for only the currently active schematic:

Type a name in the Library Name text box.  When you indicate the type of file to be added (Symbol, Package, or both) by clicking in the box for the respective file type, this will add the default extension to the file name.  Click Add Local. The library will be inserted above the currently selected library.

Schematics will automatically reload with the new library file when you exit the Editor Configuration dialog.

To change the name of an already configured library file:

Select the library file name from the list, enter a new name, and click Change.

To remove a library file from the list:

Select an existing library file and click  Delete.

Browse
Displays the File Open dialog which lets you browse the directory structure and select a file name.  After selecting a file and pressing OK, be sure to click on Add* or Add Local to add the library to the list of configured libraries.

Page Settings
Changes the default settings for each of the standard page sizes supported by Schematics, set the pin-to-pin spacing, and specify the border symbol name.

In the Editor Configuration dialog under the heading Page Settings: Drawing Area, Pin-to-Pin Border, you will notice a list of various drawing sizes (A, B, C, D, etc.) and the default dimensions for each page size.  To modify any of the pages settings, first select a setting from the list.  Next, click Page Settings and the Page Settings dialog will appear.  Enter the new width and length in inches.

Dialog Box Options

Pin-to-Pin spacing
Sets the pin-to-pin spacing to increase or decrease the size of symbols when printed.  Increasing the distance between pins (the default is 0.1 for US paper sizes, and 2.5mm for metric paper sizes) causes the symbols to appear larger when printed, relative to the drawing area.

Border Symbol (optional)
Sets the name of a border symbol.  The default border type is a single line around the drawing area.  You may choose a different border symbol, if desired.  Note that you can create your own border symbols within the symbol editor.

App Settings
Displays the App Settings dialog which allows you to specify the path and options for MicroSim tools with which Schematics interfaces.

Fonts
Changes the font which is used by Schematics to draw text on schematics. You can select any TrueType font available for your system, and customize the style and size.  A sample of the selected font is shown on the dialog.

Note that the font selected from this dialog will be used for all open documents, as well as for all subsequently-opened schematic files.


Pan & Zoom Command (Options Menu)

Sets up parameters used in panning and zooming.

Dialog Box Options

Zoom

Scale Factor
Defines the factor by which the work area should be magnified or reduced when View/In or View/Out are chosen.

Fit
Defines the percentage of work area to be filled with the complete schematic when View/Fit is chosen.

Auto Pan

Enable
When checked, turns on the AutoPan feature.  AutoPan causes the visible portion of the schematic within the work area to shift in the direction of the cursor when the cursor has been positioned within the hot zone for a time greater than or equal to the Sensitivity setting.

Hot Zone Size
Defines the scale factor for computing the width of the  hot zone in which the cursor must reside to trigger the autopan response.  To set this, type a value within the range 1 <= Hot Zone <= 10 percent of the current dimensions of the visible portion of the design.  A typical value is 2%.

Sensitivity
Defines the amout of time that the cursor must remain in the hot zone before panning occurs.  A typical value is 50nsec.

Pan

Coarse Delta
Defines the percentage of axis movement when pannning by clicking on the scroll bar.  To set this, enter a value within the range 1 <= Coarse Delta <= 50 percent.  A typical value is 25%.

Fine Delta
Defines the  percentage of axis movement when pannning by clicking on the scroll bar's up/down or right/left arrows.  To set this, enter a value within the range 1 <= Coarse Delta <= 5 percent.  A typical value is 1%.


Translators Command (Options Menu)

Translators allow you to select a translator type from the list of translators.  Type in the view which you want the netlister to take on when netlisting the design.  Click  Apply to keep the translator set at the desired view.  The view will remain the same until you change it.


Restricted Operations command (Options Menu);OrCAD;netlisting;labeling
Restricted Operations Command (Options Menu)

Enables optional netlisting options.

Dialog Box Options

Connectivity via Wire Labels
If enabled, causes wires with the same label to be merged into the same net.  If disabled (the default), wires not physically connected must be connected to either global or offpage ports of the same name to be merged during netlisting.


Electrical Rules Check Command (Analysis Menu)

Performs an electrical check of the schematic before generating a netlist or running the simulator.  The Electrical Rule Check (ERC) performs a preliminary connectivity check on the schematic.  The ERC is performed only for the current level of hierarchy.  It does not descend into the hierarchy.

If ERC errors are detected, a message appears on your screen followed by a list of errors.  This list can be recalled, reviewed, and printed by selecting Current Errors from the File menu.


Create Netlist Command (Analysis Menu)

Generates a simulation netlist for the current schematic.  A netlist is the connectivity description of a circuit, showing all of the components, their interconnections, and their values.  The netlist is generated for all levels of hierarchy, starting from the top, regardless of whether you are pushed into any level of the hierarchy.

In Schematics, the TEMPLATE attribute specifies primitive parts' contributions to the netlist.  This attribute is defined when the symbol is created.

In the process of creating the netlist, buses, connectors, etc., are resolved.

Schematics creates several files with different extensions: the file with a ".net" extension contains the netlist; the ".cir" file contains simulation commands, and the ".als" file contains alias information.


Setup Command (Analysis Menu)

Sets up which analyses will be run during simulation.

Your analysis options will vary depending upon the simulator that you are using. The setup dialogs and sub-dialogs for PLogic and PSpice are described below

PLogic Analyses

PLogic simulates the timing behavior of digital devices during a transient analysis.  During an analysis, PLogic performs a detailed timing analysis, subject to the constraints specified on the devices in your circuit.   For example, flip-flops perform setup/hold checks on the incoming clock and data signals.  Any timing violations or hazards are reported in the form of messages written to the analysis output file and the Probe data file.  Refer to the "Waveform Analysis" chapter of the Circuit Analysis User's Guide, for information on timing violations and messaging.

For detailed information on the analyses described in this section, refer to the Circuit Analysis User's Guide.  Specifically, the section titled "Digital Worst-Case Timing Simulation" will be of benefit to PLogic users.

The PLogic Analysis Setup dialog allows specification of transient analysis criteria for digital-only circuits.

Dialog Box Options

Simulation Duration
Specifies the ending time of the simulation.

Timing
Specifies the propagation delay timing to be used globally as a default for the circuit.   Any device instance with the MNTYMXDLY attribute set to zero will use the global timing set in this dialog. Part instance-specific timing characteristics can be set individually, and will override the global settings.

Flip-flop Initialization
Sets the initial state of all flip-flops in the circuit.  You can initialize all flip-flops and latches to X, 0, or 1 at the beginning of the simulation.  If set to X, all flip-flops and latches will produce an X until explicitly set or cleared, or until a known state is clicked in.  If set to 0, all such devices will be cleared.   If set to 1, all such devices will be preset.

Note that the X initialization is the safest setting since real devices do not power up to a known state.  However, the 0 and 1 settings are useful in situations where the initial state of the flip-flop is unimportant to the function of the circuit, such as a toggle flip-flop in a frequency divider.  Refer to the discussions of digital device models in the Circuit Analysis User's Guide, for more information on flip-flops and latches.

Advanced Setup
Displays the Advanced Setup dialog.

Dialog Box Options

Options
Displays the Options dialog.  The Options dialog allows you to specify various analysis parameter options.  These options are discussed in detail in the  Circuit Analysis User's Guide, and the Circuit Analysis Reference Manual.

Parametric
Displays the Parametric dialog.  The Digital Parametric analysis performs a sweep analysis while varying a global parameter.  This causes PLogic to perform a series of simulations, one for each value of the global parameter.  All expressions in the circuit are re-evaluated with the new parameter value at the beginning of each run.

Temperature
Displays the Temperature dialog which allows specification of a new default temperature for the circuit.  (The default temperature for circuit analysis is 27° Centigrade.)

PLSyn Setup
Provides access to PLSyn setup options.  This button is only enabled if the PLSyn Programmable Logic Synthesis feature is installed.  Refer to the Programmable Logic Synthesis User's Guide for information on PLSyn.

PSpice Analyses

To specify the criteria for an analysis, click the button for the type of analysis.  The corresponding setup dialog will appear allowing you to enter your analysis specifications.  Because you use the Enabled box to run an analysis, you can set up criteria for a variety of analysis, but only enable the one(s) you want to run at a particular time.  The analysis parameters are saved for the schematic regardless of whether or not the analysis was run.  Each of the analysis options is discussed in detail in the Circuit Analysis Reference Manual.  The following pages discuss each of the PSpice analysis options available for setup in Schematics, and instructions on how to fill in the dialog information.

Dialog Box Options

AC Sweep
Calculates the small-signal response of the circuit (linearized around the bias point) to a combination of inputs.

Dialog Box Options

Linear
Indicates a Linear Sweep.  The frequency is swept linearly from the starting to the ending frequency.  The Total Points value will indicate the total number of points in the sweep.

Octave
Indicates sweep by octaves.  The frequency is swept logarithmically by octaves.  The Points/Octave value will indicate the number of points per octave.

Decade
Indicates sweep by decades.  The frequency is swept logarithmically by decades.  The Points/Decade value will indicate the number of steps per decade.

Note:  The whole sweep may specify only one point if you wish; the start and end frequency values can be the same.

Total Points Octave or Decade
Indicates the total number of points in the sweep.  This value must be greater than zero.

Start Freq.
Specifies the start frequency value.  This value must be greater than zero.

End Freq.
Specifies the end frequency value.  This value must be greater than zero and must not be less than the Start Freq. value.

Noise Enabled
Causes a noise analysis of the circuit to be done.  Noise analysis is done in conjunction with AC analysis, thus, an AC sweep type must be enabled.

Output Voltage
Specifies an output voltage.  Output Voltage must be entered in the format V(<net name> [,<net name>]) where <net name> must be a fully qualified net name.  It has the form such as V(sense), which is the voltage at a net, or a form such as V(a,b), which is the output voltage across two nets a and b.

I/V Source
Specifies the name of an independent voltage or current source at which to calculate the equivalent input noise.

Interval
Specifies the print interval.  Every nth frequency where n is the print interval, a detailed table is printed showing the individual contributions of all the circuit's noise generators to the total noise.  If no value is specified in this text box, then no detailed table is printed.

Load Bias Point
Specifies that a .LOADBIAS statement will be included in the circuit file, and the contents of the bias point file will be loaded.  (Normally the bias point file will have been produced by a previous circuit simulation using the Save Bias Points option.)

Save Bias Point
Causes a .SAVEBIAS statement to be included in the circuit file, and the bias point node voltages for the specified analysis (DC, OP, or TRAN) will be saved to a user specified file name.

Dialog Box Options

File Name
Name of the file to write the bias information during simulation.

NOSUBCKT
When enabled, causes the node voltages for subcircuits to be saved.

Step
Specifies the step value at which the bias point is to be saved for parametric analyses.

MC Run
Specifies the number of the Monte Carlo or worst-case analyses run for which the bias point is to be saved.

Temp
Defines the temperature at which the bias point is to be saved for temperature analyses.

DC1
Specifies the DC sweep value at which the bias point is to be saved.  Enter a value in the DC1 text box if there is only one sweep value.  If there are two sweep variables, then DC1 specifies the first sweep value.

DC2
Specifies the second sweep value at which the bias point is to be saved.

Time
Specifies the transient analysis time at which the bias point is to be saved.  If Time REPEAT (see below) is not enabled, then the next bias point greater than or equal to Time is saved.  You can set the time step interval by enabling the Time REPEAT function.

Time REPEAT
Specifies the interval (value specified as Time) at which the bias point is to be saved.  Only the latest bias point is saved, any previous times are overwritten.  Note that if Time REPEAT is not used, then the next bias point greater than or equal to Time is saved.

DC Sweep
Causes a DC sweep to be performed on the circuit.  The DC sweep analysis calculates the circuit's bias point over a range of values.

Dialog Box Options

Swept Var. Type
Selects the variable to be swept during the analysis.  The variable type selected in this frame also impacts the remaining controls in the dialog.  You may select only one variable for each sweep.  (Use Nested Sweep to perform the analysis on more than one swept variable.)

The Name, Model Type, Model Name, and Param. Name text boxes have different requirements depending on the Swept Variable Type:

With Voltage Source enabled, a name of an independent voltage source must be entered in the Name text box.  During the sweep, the source's voltage is set to the sweep value.  If you have declared a DC value for an independent source in the circuit, this value is overridden by the sweep values during analysis.  That is, if you specify a voltage of 0.2V for V1 in the schematic, but specify a sweep range of -0.125V to 0.125V the value of 0.2V will be ignored for the analysis.

With Temperature enabled, the temperature is used as the sweep variable.  For each value in the sweep, all the circuit components have their model parameters updated to that temperature.  The Name, Model, and Param text boxes are not used.

With Current Source enabled, a name of an independent current source must be entered in the Name text box.  During the sweep, the source's current is set to the sweep value.

With Model Parameter enabled, you must enter the name of a valid model type in the Model Type text box, the model name in the Model Name text box, and a parameter name in the Param. Name text box.  The parameter in the model is set to the sweep value.

With Global Parameter enabled, you must enter the name of a global parameter in the Name text box.  The parameter value is set to the sweep value.  (Global parameters can be established by placing a PARAM pseudocomponent.)

Sweep Type Parameters:

Linear
Indicates linear sweep.  The swept variable is swept linearly from the starting to the ending value.  The Increment value is the step size.

Octave
Indicates sweep by octaves.  The sweep variable is swept logarithmically by octaves.

Decade
Indicates sweep by decades.  The sweep variable is swept logarithmically by decades.

Value List
Specifies that the list of values in the Values field are the values that the sweep variable will be set to.

Start Value and End Value text boxes have different meanings depending on which Sweep Type is selected.  Start Value may be greater or less than End Value, that is the sweep may go in either direction.

Values
Specifies the list of values used when Value List is enabled.

Nested Sweep
Displays a second dialog for entry of nested sweep analysis parameters.  A second sweep variable, sweep type, start, end, and increment values may be placed after the first sweep.  In this case, the first sweep will be the inner loop: the entire first sweep will be done for each value of the second sweep.  The rules for the values in the second sweep are the same for the first.

Monte Carlo/Worst Case
Varies the lot or device tolerances of devices between multiple runs of an analysis (DC, AC, or transient).  Before running the analysis, you must set up the device and/or lot tolerances of the model parameter(s) to be investigated.   You may specify either a Monte Carlo or a worst-case analysis.

Dialog Box Options

Monte Carlo
Monte Carlo causes a Monte Carlo (statistical) analysis of the circuit to be performed.  When Monte Carlo is selected, the MC Runs text box indicates the total number of runs for the analysis.

Worst Case
Specifies that a sensitivity and worst-case analysis of the circuit to be performed.

Analysis Type
Specify for which type of analysis the Monte Carlo or Worst Case analysis is to be done:  AC, DC, or Transient analysis.

Multiple runs of the selected analysis are done while parameters are varied.  You can select only one analysis type (AC, DC, or Transient) per run.  The analysis selected will be repeated in subsequent passes of the analysis.

Output Variable
Must be entered in the format V(<net name> [,<net name>]), where <net name> must be a fully qualified net name.  It has the form such as V(sense), which is the voltage at a net, or a form such as V(a,b), which is the output voltage across two nets a and b.

Function text boxes and option buttons specify a function to be performed on the values of the output variable to reduce them to a single value.  You can specify one of the following:

YMAX
Finds the greatest difference in each waveform from the nominal run.

MAX
Finds the maximum value of each waveform.

MIN
Finds the minimum value of each waveform.

RISE
Finds the first occurrence of the waveform crossing above the threshold value.  Enter the threshold value in the Rise/Fall text box.

FALL
Finds the first occurrence of the waveform crossing below the threshold value.  Enter the threshold value in the Rise/Fall text box.

Range Lo
Specifies the lower limit of the range over which the function will be evaluated.

Range Hi
Specifies the upper limit of the range over which the function will be evaluated.

MC Options
Specify the analysis constraints of a Monte Carlo analysis as follows:

None
Only the nominal run produces output.

All
Forces all output to be generated (including the nominal run).

First
Generates output only during the first n runs.  Enter the value for n in the Value text box.

Every
Generates output every nth run.  Enter the value for n in the Value text box.

Runs
Generates output only for listed runs.  Up to 25 values may be specified in the Value text box.

List
Specifies that, at the beginning of each run, the model parameter values actually used for each component during that run.

Seed
Defines the seed for the random number generator within the Monte Carlo analysis.  You must enter an odd integer ranging from 1 to 32767.  If the seed value is not set, it will explicitly default to 17533.

Worst-Case Options
Specify the analysis constraints of a Worst-case analysis as follows:  .

Output All
Requests output from the sensitivity runs, after the first run.  The sensitivity and worst-case runs are done with variations on model parameters as specified by the DEV and LOT tolerances.  The default is to vary by BOTH.

List is used to limit the devices considered to only those device types listed  in the Devices text box.  List consists of a string containing the initial letters of those PSpice primitives that are to be included in the analysis.  For example, the string QRC would include only bipolars, resistors, and capacitors

Note:  You can run either a Monte Carlo or worst-case analysis, but not both at the same time.

Bias Point Detail
When enabled in the Analysis/Setup dialog, writes the detailed bias point information to the simulation output file.

The information reported to the output file consists of the following:

·	A list of all the analog node voltages

·	A list of all the digital node voltages

·	The currents through all the voltage sources, and their total power

·	A list of the small-signal parameters for all the devices

Digital Setup
Displays the Digital Setup dialog for specifying a transient analysis on a digital or mixed-signal circuit.

Dialog Box Options

Timing
Specifies the propagation delay timing to be used globally as a default for the circuit.   Any device instance with the MNTYMXDLY attribute set to zero will use the global timing set in this dialog. Part instance-specific timing characteristics can be set individually, and will override the global settings.

Flip-flop Initialization
Sets the initial state of all flip-flops in the circuit.  You can initialize all flip-flops and latches to X, 0, or 1 at the beginning of the simulation.  If set to X, all flip-flops and latches will produce an X until explicitly set or cleared, or until a known state is clicked in.  If set to 0, all such devices will be cleared.   If set to 1, all such devices will be preset.

Note that the X initialization is the safest setting since real devices do not power up to a known state.  However, the 0 and 1 settings are useful in situations where the initial state of the flip-flop is unimportant to the function of the circuit, such as a toggle flip-flop in a frequency divider.  Refer to the discussions of digital device models in the Circuit Analysis User's Guide, for more information on flip-flops and latches.

Default A/D Interface
Controls the generation of intermediate R, F, and X levels through analog/digital interfaces.

Level 1 generates the intermediate values, and Level 2 does not.  (Level 3 and Level 4 are seldom used.)  Refer to the "Analog/Digital Interfaces" chapter of the Circuit Analysis User's Guide for more information.

In general, if you are performing a digital worst-case timing analysis, you should use Level 1.

Options
Sets a variety of factors that control the accuracy of your results.  The defaults are initially displayed for each item.

To change a Y/N option:
Select an option, then double-click to toggle the item to Y for yes, or N for no.

To change the value of an option
Select the option.  The current value will appear in the New Value text box.  Enter the new value and click Accept to confirm.

Parametric
Performs a parametric sweep analysis on a sweep variable name, for all of the analyses of the circuit.  Parametric does not allow nested sweeps.  You may not specify a DC Sweep and a Parametric analysis for the same variable

Dialog Box Options

Swept Var. Type
Selects the variable to be swept during the analysis.  The variable type selected in this frame also impacts the remaining controls in the dialog.  You may select only one variable for each sweep.  (Use the Nested Sweep option in the DC Sweep analysis to perform an analysis with more than one swept variable.)

With Voltage Source enabled, a name of an independent voltage source must be entered in the Name text box.  During the sweep, the source's voltage is set to the sweep value.

With Temperature enabled, the temperature is set to the sweep value.  For each value in the sweep, all the circuit components have their model parameters updated to that temperature.

With Current Source enabled, a name of an independent current source must be entered in the Name text box.  During the sweep, the source's current is set to the sweep value.

With Model Parameter enabled, you must enter the name of a valid model type in the Model Type text box, the model name in the Model Name text box, and a parameter name in the Param. Name text box.  The parameter in the model is set to the sweep value.

With Global Parameter enabled, the global parameter's value is set to the sweep value and all expressions are re-evaluated.  Enter the global parameter name in the Name text box.

Sweep Type Parameters:

Linear
Indicates a linear sweep.  The swept variable is swept linearly from the starting to the ending value.  The Increment value is the step size.

Octave
Indicates sweep by octaves.  The sweep variable is swept logarithmically by octaves.

Decade
Indicates sweep by decades.  The sweep variable is swept logarithmically by decades.

Value List
Uses a list of values.  In this case there are no start and end values.  Instead, the numbers that are listed in the Values text box are the values that the sweep variable will be set to.

Start Value and End Value
Will vary depending upon which sweep variable type you select.  The Start Value may be greater or less than the End Value.

Increment
For Linear sweep type, specifies the step increment to be calculated within the start and end frequency values.  If an Octave or Decade sweep variable is selected, Increment indicates the number of points per octave or decade.

Values
Specifies the list values if Value List sweep type is selected.  This list of values should be listed in ascending or descending order.

Sensitivity
Causes a DC sensitivity analysis to be performed. One or more output variables may be specified. The <output variable>, if it is a current, is restricted to be current through a voltage source.

Device sensitivities are provided for the following device types only:

·	resistors,

·	independent voltage and current sources,

·	voltage and current-controlled switches,

·	diodes,

·	bipolar transistors.

Temperature
Specifies the temperature or list of temperatures at which all analyses are performed.  The temperatures are in degrees Centigrade.  If more than one temperature is given, then all analyses are done for each temperature.

You can enter either a single value for the Temperature text box, or a list of temperatures.  When a list is entered, the circuit is simulated multiple times, once for each temperature in the list.  Note that running an analysis at multiple temperatures can also be done as a parametric analysis.  With parametric analysis, the temperatures may be specified either by list or by range and increments within the range.

The default temperature for simulation is 27 degrees Celsius.

Note:  The statistical analyses perform multiple runs, as does the Temperature analysis when a temperature range is entered.  Conceptually, the Monte Carlo and worst-case loops are inside the Temperature loop.  However, since both temperature and tolerances affect the model parameters, the interaction of the two may become complicated. Therefore, we recommend not using the Temperature analysis option to sweep multiple temperatures when using Monte Carlo or worst-case analyses in a circuit.  For the same reason, we do not recommend sweeping the temperature with a DC Sweep analysis while performing one of these statistical analyses.  We also do not recommend putting tolerances on temperature coefficients.

Transfer Function
Causes the small signal transfer function to be calculated by linearizing the circuit around the bias point.

Dialog Box Options

Output Variable
Specifies an output voltage or current through a voltage source.  The Output Variable must be entered in the format V(<net name> [,<net name>]) or I(<voltage source name> [,<net name>]) where <net name> must be a fully qualified net name.  For example, V(a,b), specifies the output voltage across two nets a and b, and I(VDRIV) specifies the current through a voltage source VDRIV.

Input Source allows you to specify the name of a voltage or current source.

Transient
Calculates the behavior of the circuit over time, starting at TIME = 0 and going to the final time value.

Dialog Box Options

Print Step
Specifies the time interval used for printing or plotting the results of the transient analysis.  (This parameter refers only to the results written to the output file.  This has no effect on the Probe data file.)

Final Time
Specifies the ending time for which the circuit's behavior is calculated.

No-Print Delay
Specifies the length of time, from TIME = 0, which is not printed, plotted, or output to Probe.

Step Ceiling
Specifies a ceiling smaller or larger than the print interval to be put on the internal time step.  During analog simulation, the simulator maintains an internal time step which is continuously adjusted to maintain accuracy while not performing unnecessary steps.  During periods of inactivity, the internal time step is increased, and during active regions, it is decreased.  The maximum internal step size can be controlled by specifying the Step Ceiling value in the dialog.  The simulator will never exceed either the step ceiling value or two percent of the total transient run time, whichever is less.

Detailed Bias Pt
When enabled, sends output to the ".out" file.

Skip initial transient solution
When enabled, causes the transient analysis to skip the bias point calculation and proceed directly with analysis at TIME=0.  Initial conditions set on capacitors and inductors using the IC attribute, or using IC1 and IC2 symbols, still take effect; however all other such devices are assumed to have an initial value of 0.  See the "Setting Initial Conditions" section in the "Analog and Digital Parts" chapter of the Circuit Analysis User's Guide for more information.

Fourier Analysis Parameters:

With Fourier analysis enabled, a decomposition into Fourier components of the result(s) of a transient analysis is performed.  A Fourier analysis requires a transient analysis.

Center Frequency
Specifies the fundamental frequency value.

Output Vars
Specifies an output voltage or current output variable of format V(<net name> [,<netname>]), and <net name>'s must be fully qualified.


Library and Include Files Command (Analysis Menu)

Specifies the  Model Library, Include, and Stimulus Library files to be included in the simulation netlist.  Library, include, and stimulus files may be designated for inclusion either globally or on a schematic-specific basis.  Each schematic can have its own unique list of files.  Library files will be inserted in the netlist with a .LIB command.  Include files will be inserted in the netlist with a .INC command.  Stimulus library files will be inserted in the netlist with a .STMLIB command.

The Library and Include Files dialog displays three list boxes displaying all of the library, include, and stimulus library files specified, one file per line.  Note that the list boxes can contain two kinds of files; global and local (to the schematic).  Global files are the files listed in .LIB and .INC lines in the [SCHEMATICS NETLIST] section of "msim.ini," and are marked with an asterisk (*) after the file name.  These files are included in every schematic.  The local library, include, and stimulus library files will be available only for the current schematic.

To add a library or  file reference to the current schematic only:
Enter the file name in the File Name text box, and click on the Add Library, Add Include, or Add Stimulus button.  This stores the file name locally with the current schematic and the file will only be included in the current schematic's netlist.

To add a global library or file reference to every schematic netlist sent to the simulator:

Enter the file name in the File Name text box.  Click on the Add Library*,  Add Include*, or Add Stimulus*  button.  This will make the file name available to all schematics by storing it in the "msim.ini" file.

To remove a library, include or stimulus file:

Select the file name then click Delete.  The file will be removed from the list.

Note:  All parts in the standard Model Library are accessible if there is a "nom.lib" entry under Library Files.  If you remove this entry, be aware that you will need to add a "bipolar.lib" entry to access small-signal bipolars, a "jfet.lib" entry to access junction FETs, and so on.

To change the name of a library, include or stimulus file:

Select a file name from either of the list boxes, make your modifications in the File Name text box, then click Change.

Browse allows you to browse the directory structure and select a file name.  The File/Open dialog will appear allowing you to search through the available directories for a file name.  Once the file name is selected, click on one of the add buttons to accept the new file name.

When the Create globally unique instance model name option is enabled, Schematics searches all libraries configured for the current schematic when creating a unique name for a new model.  This is not necessary if all user-customized models are saved in a local library, especially if they are saved in the "<filename>.lib" file for the schematic.  By default, this option is not enabled so that only local libraries are searched when creating a new name for a new instance model.  Disabling this option makes editing models much quicker


Simulate Command (Analysis Menu)

Performs a PSpice or PLogic circuit analysis on the current schematic.  This command automatically performs the following, if necessary: annotation, Electrical Rule Check (ERC), and netlist generation.

The simulation creates output files with a ".out" extension, and if the simulation completes successfully, produces a file with a ".dat" extension.  The output (".out") file contains bias point information, model parameter values, etc.  This is a text file which you can view by choosing Examine Output from the Analysis menu.  The ".dat" file is the data file containing the simulation results to be displayed by Probe.  All viewpoint and sensor displays are automatically updated.

Note:  If you have edited a symbol in the Symbol Editor, you will need to re-create the netlist before simulating for any changes to be relevant to the netlist.  For example, if you change the TEMPLATE attribute on a part, then return to the Schematic Editor and make no other modifications, you need to select Analysis/Create Netlist to force the creation of a new netlist (which includes edits made to the TEMPLATE attribute), then select Simulate.


Probe Setup Command (Analysis Menu)

Displays a dialog which allows you to specify how the Probe waveform analyzer will be run during simulation.

Probe Setup settings are stored with each schematic.

Dialog Box Options

Automatically Run Probe After Simulation
Causes Probe to be automatically invoked after the simulation has been completed.

Monitor Waveforms (Auto-Update)
Causes Probe to be started when the simulator is started so that waveforms are updated as the simulation progresses.  (Available only for the PC/Windows platform.)  If this option is grayed out, disable the Text Data File Format (CSDF) check box.

Do Not Auto-Run Probe disables automatic invocation of Probe.

At Probe Startup Parameters:

Restore Last Probe Session
Restores the display using the display control setup from the previous Probe session.

Show All Markers
Displays traces corresponding to all markers located on the schematic.

Show Selected Markers
Displays traces for the markers selected on the current page of the schematic.

None
Does not display any traces automatically.

Data Collection Parameters:

At Markers Only
Saves the Probe data only at those nodes and devices where markers are placed.

All
Saves Probe data for all nodes and devices in the circuit.  This is the default.

All Except Subcircuit Data
Saves data for all nodes and devices, except internal subcircuit nodes and devices.

None
Disables Probe data collection

Text Data File Format (CSDF)
When enabled, writes Probe data in text format rather than binary format.  This option is not available if the Run Probe During Simulation option is used.


Run Probe Command (Analysis Menu)

Lets you examine the results of a PSpice simulation using the Probe graphical waveform analyzer.  You can set up Probe to run automatically after each PSpice simulation, by checking the box in the Probe Setup command dialog.


Examine Netlist Command (Analysis Menu)

Displays the simulation netlist file using the configured text editor (Notepad is the default)  You can examine the file but you should not modify it.  You can reconfigure the text editor used by editing "msim.ini."  For information on modifying "msim.ini," see "Appendix A" in the Installation Manual.

Note:  Notepad has a file size limit of 64 kilobytes.


Examine Output Command (Analysis Menu)

Displays the output file (".out"), which is created by running the simulator. When you select Examine Output, the current output file appears.  You can examine the file, but you should not modify it.


Annotate Command (Tools Menu)

Assigns reference designators to parts, or deletes previous annotations.

Dialog Box Options

Package and Assign Reference Designators
Packages individual parts into physical packages based on the package definition information for the part.  If enabled, this will assign reference designator, gate, and package type annotated attributes to parts based on what you have specified in the Set Values frame.  The entire design will be packaged.

Assign Reference Designators Only
Assigns unique reference designators to each part instance.  Reference designators will be assigned to parts based on what is specified in the Set Values frame.  Reference designators will only be assigned for parts on the current schematic.   No packaging is done.

Undo Annotation
Removes any annotated attributes, (i.e., any attributes that were added via the Back Annotate command, through packaging, or that have been added to schematic instances, see Navigate/Edit Schematic Instance).  Reference designators assigned when parts are placed via Auto-Naming are not cleared.

Set Values f
Specifies which parts will have reference designator and/or package information assigned.

All Except User-Assigned
Restricts the function to those attributes that have not been manually assigned by the user (via the Edit/Attribute command).

Only Unassigned
Restricts the function to values for reference designator, gate, and package type attributes that have not yet been assigned.

All
Gives the function unrestricted access to all parts, overriding user-assigned attribute values.

Starting Designator
Specifies the number of the first reference designator to be assigned.

Page Increment
Specifies the amount to add to the starting designator between pages of the schematic.

Level Increment
Specifies the amount to add to the starting designator between levels of hierarchy.

Package Class Priorities
Provides the current list of classes that will be used to assign a package type for a part.  For each package to be assigned a package type, the packager will go through the package classes in the order listed, and assign the first package type defined for that part which belongs to that class.  However, if only one package type is  defined for the package, it will be used, whether it is in the list or not.

Setup Priorities
Modifies the list of package class priorities used by the packager to assign package types.  This brings up the Setup Priorities dialog.


Create Layout Netlist Command (Tools Menu)

Generates a layout netlist in the currently selected layout editor format.   A layout netlist consists of part and connectivity information needed by the layout editor.


Run Layout Editor Command (Tools Menu)

Starts the currently configured layout editor (assuming that it runs under your operating system).


Back Annotate Command (Tools Menu)

Back annotates a schematic using an ECO file generated by the layout editor.


Configure Layout Editor Command (Tools Menu)

Selects the layout editor format to be used.

Dialog Box Options

Netlist File Extension
Specifies the default netlist file extension for the selected layout editor.

ECO
Specifies the default file extension for an ECO file from the selected layout editor.

Command Line
Specifies the command to invoke the selected layout editor.  Note that the editor must be compatible with your operating system.  The following special sequences may be included in the command line:

%c	current working directory

%e	schematic name without extension

%f	entire name

%n	schematic name without extension or path

For example, if the file "c:\msim\example.sch" is the currently loaded schematic, then the following text is substituted in the command line in place of the special codes:

%c	c:msim

%e	c:\msim\example

%f	c:\msim\example.sch

%n	example


Browse Netlist Command (Tools Menu)

Displays the current layout netlist using the configured text editor.  You can select a different text editor by editing "msim.ini" (refer to Appendix A of the Installation Manual).


View Package Definition Command (Tools Menu)

Displays the package definition for the currently selected part.  For a detailed discussion on all the items in the Package Definition dialog


Create Subcircuit Command (Tools Menu)

Creates a subcircuit netlist for the current level of hierarchy and all lower levels.  This netlist will be written to "<schematic name>.sub" (not the usual ".net" file).  At the current level of hierarchy, interface ports will be mapped into subcircuit interface nodes.  Note that if you have made changes to the current level, you should save the changes before invoking the Create Subcircuit command.


Run Polaris Command (Tools Menu)

Invokes the Polaris signal integrity configuration dialog, if Polaris is present.  This menu item is only available if you have the Polaris Signal Integrity package.  Refer to the Signal Integrity User's Guide for information on setting up and using Polaris.


Run PLSyn Command (Tools Menu)

Invokes the PLSyn Programmable Logic Synthesis configuration dialog, if PLSyn is present.  This menu item is only available if you have the PLSyn Programmable Logic Synthesis package.  Refer to the Programmable Logic Synthesis User's Guide for information on setting up and using PLSyn.


Run PSpice Optimizer Command (Tools Menu)

Invokes the Circuit Optimization configuration dialog.  This menu item is only available if you have installed the PSpice Optimizer software option.  Refer to the Analog Performance Optimization User's Guide for information on the PSpice Optimizer.


Use Optimized Parameters command (Tools Menu)
Use Optimized Params Command (Tools Menu)

Sets the value for each optimizer parameter to the values that were back-annotated from a previous PSpice Optimizer run.  This menu item is only available if you have the PSpice Optimizer software option.


Mark Voltage/Level Command (Markers Menu)

Lets you place a marker to show the voltage or digital signal at a net.  These markers must be placed on wires or at a pin.


Mark Voltage Differential Command (Markers Menu)

Lets you place markers to show the voltage difference between two nets.  Voltage Differential markers consist of a pair of objects, one for the `+' node and one for the`-' node.  Each object must be placed on a bus, wire, or at a pin.


Mark Current into Pin Command (Markers Menu)

Lets you place a marker to show the current into a terminal of a three or four terminal device, (such as a Bipolar transistor, MOSFET, JFET, or GaAs MESFET), or the current through a two terminal device, (including inductors, resistors, capacitors, and  diodes, among others).  If placed on an incompatible device, a warning will be given and the marker will be ignored.


Mark Advanced Command (Markers Menu)

Displays a list of the available symbols in the Marker Symbol Library file "marker.slb."  Refer to the Circuit Analysis User's Guide for a description of the types of marker symbols available.


Clear All Command (Markers Menu)

Deletes all markers on all pages of the schematic.


Show All Command (Markers Menu)

Updates Probe with waveforms for all markers on all pages.


Show Selected Command (Markers Menu)

Updates Probe with waveforms for all currently selected markers.


New Window command (Window Menu)
New Command (Window Menu)

Opens another occurrence of the current window.  This allows you to view different areas of the same schematic file simultaneously.  Because these windows are just different views of the same file, all changes made in one of the windows will be reflected in the other.


Close Command (Window Menu)

Closes the current document window.  If it is the only window for a schematic file, you will be prompted to save any changes that have been made before closing.  If there are other open windows for the same schematic file, then no prompt is displayed.


Arrange Command (Window Menu)

Displays a dialog which allows you to select an arrangement for all of the open windows.

Dialog Box Options

Tile
Arranges all of the open windows in a tiled arrangement (that is, with no overlap).  Depending on the number of windows, they may be tiled horizontally, vertically, or a combination of both.

Tile Horizontal
Arranges all of the open windows in a tiled arrangement, maximizing the width of each window where possible.  A combination of horizontal and vertical tiling may be used depending on the number of windows.

Tile Vertical
Arranges all of the open windows in a tiled arrangement, maximizing the height of each window where possible.  A combination of vertical and horizontal tiling may be used depending on the number of windows.

Cascade
Arranges all of the open windows in a stacked arrangement.


New Command (Symbol Editor File Menu)

Creates a new symbol library


Open Command (Symbol Editor File Menu)

Loads an existing Symbol Library file for editing.  Select the directory in which your Symbol Library files are stored.  The default directory will automatically appear with the list of Symbol Library files it contains.  Select a ".slb" file from the list and click OK to open it.


Close Command (Symbol Editor File Menu)

Closes the current Symbol Library file.  If the file has not been saved, you will be prompted to save the changes before the window is closed.


Save Command (Symbol Editor File Menu)

Saves the updated Symbol Library file to its present file name.  If there is no current library file name, you will be prompted for one.  The previous version of the Symbol Library file is copied to your backup directory.


Save As Command (Symbol Editor File Menu)

Saves the updated library file to a new file name.  A dialog will appear and prompt you for the file name.


Print Command (Symbol Editor File Menu)

Prints one or more symbols.

Dialog Box Options

Current Printer
Shows the current default printer.  The printer can be changed through the Printer Select button (see below) or through the File/Printer Select command.

Parts
Lists the parts in the current library.

Current Symbol Only
When enabled, prints only the symbol that is currently being edited.

Select All Parts
Selects all parts in the current library file to be printed.

Symbol Image
When enabled (the default), prints the graphics of the selected symbol(s) on the hard copy.

Attributes
When enabled (the default), lists all of the attributes and their values for the selected symbol(s) on the hard copy.

Symbol Data
When enabled (the default), lists the symbol description, type, Bbox dimensions, and origin position on the hard copy.

Pin Data
When enabled (the default), lists the pin data of the selected symbol(s) on the hard copy.

Auto-Fit: one symbol per printer page
When enabled, expands each symbol to full page size.

User-definable zoom factor (%)
When enabled (the default), allows you to set the zoom factor for the size of the symbol on the printed page.

Page Setup
Invokes the Page Setup dialog for setting the margins for the printed page.  Margin defaults are 1/2" or 15mm.  Setting up different margins modifies the area the schematic page will occupy if Auto-fit is selected.  If User-definable zoom factor is selected, the drawing will be the specified size, but offset by the margin values.

Printer Setup
Displays the setup options for the currently selected printer.  This dialog will vary depending on the printer that you are using.

Printer Select
Selects  another printer.  This displays the same Printer Select dialog as the File/Printer Select command.


Printer Select Command (Symbol Editor File Menu)

Selects a printer to use with the Symbol Editor and set up printing options.   Once you have selected a printer from the list, use Setup to display the configuration options for your particular printer.  Your printer configuration for the Symbol Editor will stay the same until it is modified again through the Setup command.  The printer configuration is independent of other applications' printer configurations.  Set up the printer the way you wish, and click OK when you are finished to copy the printer setup to "msim.ini."


Current Errors Command (Symbol Editor File Menu)

Display the  list of the recently logged errors and allows you to view, print, or save them to a file.


Exit Command (Symbol Editor File Menu)

Exit quits Schematics.


Undelete Command (Symbol Editor Edit Menu)

Restores the last object(s) deleted and removes it from the buffer.


Cut command (Symbol Editor Edit Menu)
Cut Command (Symbol Editor File Menu)

Deletes the selected item(s).  The deleted item remains in a buffer for use with the Paste or Undelete commands.  The Cut command retains only the last item (or set of items) in the buffer.


Copy command (Symbol Editor Edit Menu)
Copy Command (Symbol Editor File Menu)

Copies the selected object(s) to a buffer for use with the Paste command.  The Copy command retains only the last item (or set of items) in the buffer.


Paste command (Symbol Editor Edit Menu)
Paste Command (Symbol Editor File Menu)

Retrieves the last item (or set of items) stored in the buffer from the Cut or Copy commands for placement.


Delete command (Symbol Editor Edit Menu)
Delete Command (Symbol Editor File Menu)

Deletes the selected items.  The deleted items can be restored with the Undelete command.  The paste buffer is not affected.


Change command (Symbol Editor Edit Menu)
Change Command (Symbol Editor File Menu)

Edits selected text, pins, or attributes associated with a symbol.  You can also edit these items without using the menu by double-clicking on the desired item.  For any text, pin, or attribute you select to edit, a separate dialog will appear for that item.

Changing Text

If text is selected, the Change Text dialog shown above will appear.  This dialog allows you to type in the text, specify the relative font size, the orientation of the text, and its horizontal or vertical justification.  Text allows you to edit the selected text.  A dialog appears allowing you to type in the desired text.

Changing Pins

If pins, pin names, or pin attributes are selected, the Change Pin dialog appears showing the default values for the pin description.

Note:  Use the Pin List command if you wish to edit all pins as a group.

Pin Name
Pin identifier, and is required.  It can also be used to define the number of signals that must be contained in a connecting wire or bus.

Display Name
Acts as a toggle to turn the visibility of the pin name on or off.

Type
Determines how the pin will be displayed on the schematic.  The default is normal, which is a 10-unit line segment.

Hidden
Set a pin to be invisible in the Schematic Editor.  If you set the visibility off, you must supply the name of a connecting net (normally a global net like $G_DPWR or $G_DGND) for this pin in the Net text box.  This net is recorded as a symbol attribute (not a pin attribute).  The IPIN(<pinname>)=<net name> attribute conveys the net name.

Net
Specifies the name of the net to which a hidden pin will be connected in the Schematic Editor.  Enter the name of the connecting net in the Net text box.

The Change Pin dialog also allows you to specify the associated pin number and set the type of pin.  These settings can be found under the "Pin Attributes" section of the Change Pin dialog.

Pin
Specifies the pin number.  In a multi-gate part, this generally corresponds to the appropriate pin number on the first gate.

ERC
Defines the type of pin used for electrical rule checking in the Schematic Editor, and defaults to don't care.

Modeled Pin
Indicates that this is a modeled pin.  If the pin is not part of the simulation model (such as balance and offset pins on some opamps) then the box should be unchecked.  When the box is unchecked, the pin is marked as not simulated and a FLOAT=u attribute is applied to the pin.  This allows the netlister to pay special attention to the pin of there are fewer than two connections at its node.  If that is the case, a resistor to ground is added for simulation.

If the Modeled Pin checkbox is not marked, the Float list box (below) is disabled.

Float
Provides a list box that allows you to select a default action that the simulation netlister will take if the pin is unconnected.  The choices are as follows:

RtoGND	add a large resistor to ground for the pin

UniqueNet	generate a unique node to monitor with a Probe marker

Error	cause netlister to fail and generate Unconnected Pin error

Edit Attributes
Edits the pin attributes.  Click Edit Attributes in the Change Pin dialog.   This dialog lets you change whether pin numbers are to be shown.


Pin Type command (Symbol Editor Edit Menu)
Pin Type Command (Symbol Editor File Menu)

Changes the display type of any selected pins, or, if no pins are selected, sets the default pin display type for new pins.


Model command (Symbol Editor Edit Menu)
Model Command (Symbol Editor File Menu)

Lets you edit the simulation .MODEL or .SUBCKT definition for a part.  From within the Symbol Editor, the global model or subcircuit representation is edited.  By default, these changes are saved in a file called "user.lib."  Changes made to the model or subcircuit in the Symbol Editor will affect all the parts that use this model or subcircuit.

When editing an existing model the default Model Name is the original name of the model found.  The default library file name will be "user.lib."  Note that this is a different default library file name than the one offered in the Schematic Editor.  (This is in keeping with the idea that the changes made in the Schematic Editor should be associated with the schematic.  Changes made in the Symbol Editor are to the actual model or subcircuit definition of the symbol, and are global.)  Make all modifications as necessary in the text edit work area, enter a new library file name if desired, and click on OK to accept the definition.

Edit Model (Text) displays the Model Editor dialog with a copy of the model or subcircuit definition associated with that part, if one exists.  Otherwise, you will be presented with a blank edit dialog in which you can create a new model or subcircuit definition.

Note that you must use the text-based model editor to edit any model type which is not supported by the Parts program, and to add Monte Carlo parameters.

To create a new model or subcircuit definition, simply begin typing in the definition in the text edit work area.  Click the mouse inside the text edit work area to activate the cursor.  To enter a model definition, the required format is:

.MODEL <model name> [AKO: <reference model name>] <model type> (

<parameter name> = <value> [tolerance specification]

<parameter name> = <value>)

For example:

.model  rmax  res (

R=1.5

TC1=.02

TC2=.005)

or when adding AKO references and tolerance specifications:

.model  q2n222-x npn AKO: q2n222 (

is=14.34f

Xti=3

rb=10 dev 10%)

(See the Circuit Analysis Reference Manual for syntax on the .MODEL and .SUBCKT statements.)

Enter the library file name in the Library text box, then click on OK to accept the model definition and exit the dialog.

Expand AKO will search through any AKOs the model might have and add these new parameters to the model.  This command essentially flattens a hierarchy of AKOs into one model definition where you can see all the parameters.

Edit Model (Parts) (Windows only) invokes the Parts program for graphical editing of the model parameters.  This option may be used to edit models which are supported by the Parts program.  (Refer to the Circuit Analysis User's Guide for information on the Parts program for Windows.)

If a customized model already exists for this part, then it is loaded from "user.lib" for editing with the Parts program.  If no custom model exists, then the model is copied from the original library.  The edited model is then saved to the "user.lib" file.


Stimulus command (Symbol Editor Edit Menu)
Stimulus Command (Symbol Editor File Menu)

Invokes the Stimulus Editor when a stimulus symbol is currently selected.  Refer to the Circuit Analysis User's Guide for information on using the StmEd program.


Push command (Symbol Editor Edit Menu)
Push Command (Symbol Editor File Menu)

Displays the subschematic represents by the symbol.  If no schematic has been created for the symbol, the Schematic Editor will appear with a blank screen, (a new schematic).  Interface ports will be added automatically with their labels corresponding to symbol pin names.  If the symbol represents only one schematic, the Schematic Editor is invoked on that schematic, and edits to the schematic can be made.

If the symbol represents more than one schematic, the Push dialog appears allowing you to choose which schematic to bring up for editing in the Schematic Editor.  The symbol name will be given, as well as a list of view name/schematic name pairs.  Select the pair with the schematic name that you want to edit, and click OK.  The Schematic Editor will be invoked on the schematic you chose from the list.


Set Schematic command (Symbol Editor Edit Menu)
Set Schematic Command (Symbol Editor File Menu)

Sets the schematic name or edit a list of schematics that the symbol will represent, as well as set up the schematic view names.  If there is only one, or no schematic that a symbol currently represents, the symbol can be set to represent a schematic through the dialog.  Enter the schematic name in the dialog and click OK to establish the relationship.

Click Set Views to set up the view name for each schematic that the symbol represents.  You can set up multiple views for one schematic.  If the symbol represents more than one schematic, the Set Views dialog appears directly.


Check Schematic command (Symbol Editor Edit Menu)
Check Schematic Command (Symbol Editor File Menu)

Checks the interface and global ports, and global nets implied through hidden pins on the schematic(s) that the current symbol represents, against the pins and hidden pins in the symbol.  Changes cannot be made to schematics from the Symbol Editor.  You will need to go into the Schematic Editor and make any necessary modifications.


Rotate command (Symbol Editor Edit Menu)
Rotate Command (Symbol Editor File Menu)

Rotates a selected object(s) 90 degrees counterclockwise.  If you select an area of your schematic, the area is rotated around the center of the ROI box.


Flip command (Symbol Editor Edit Menu)
Flip Command (Symbol Editor File Menu)

Flips a selected object(s) about the Y axis to produce a mirror image of the object.


Align Horizontal command (Symbol Editor Edit Menu)
Align Horizontal Command (Symbol Editor File Menu)

Moves all selected objects (lines, wires, arcs, circles, text, etc.) so that their origins are along the same horizontal line.  Objects are aligned with the topmost object..


Align Vertical command (Symbol Editor Edit Menu)
Align Vertical Command (Symbol Editor File Menu)

Moves all selected objects (lines, wires, arcs, circles, text, etc.) so that their origins are along the same vertical line.  Objects are aligned with the leftmost object.


Arc Command (Symbol Editor Draw Menu)

Adds an arc to the symbol.  To begin, click to select an end-point of the arc.  Click again to select the other end-point.  Then, as you move the mouse, you will see the arc-shape formation.  When the arc is the desired size, click to fix the arc at that position.


Box Command (Symbol Editor Draw Menu)

Adds a rectangle to the symbol.  To begin, click to select a location for the upper left corner of the box.  As you drag the mouse, the shape and size of the box changes.  When the box is the desired size, click to finish drawing the box.


Circle Command (Symbol Editor Draw Menu)

Adds a circle to the symbol.  To begin, click to select the center of the circle.  Then move to extend the of the circle.  As you move, the new circle is drawn with the cursor used as a point on the perimeter of the circle.  Click to set the circle at the desired size.


Line Command (Symbol Editor Draw Menu)

Adds a line to the symbol.  Once in this mode, the cursor changes to a pencil-shape while you re

drawing.  To begin, click at the starting point for the line.  Move the cursor to extend the line, and click to set a vertex, or double-click to end the line.


Pin Command (Symbol Editor Draw Menu)

Adds a pin to a symbol.  This command is modal; while in this mode, the cursor changes to the outline of a pin.  Move the pin outline to the desired location and click to place the pin.  A small `x' appears on one end which marks the connectivity point of the pin.  You can add additional pins by clicking at the desired locations.  Double-click to place the current pin and end the mode.  Right click to end the mode without placing the current pin.

Note:  When you choose Graphics/Pin, the pin type will default to whichever type was last placed or to the type defined under the Pin Type command. For example, if you changed the pin to an inverted clock type using the Pin Type command, each pin you place after that will be an inverted clock pin.  The pin will remain an inverted clock type until you select a new pin type with the Pin Type command, or change the pin type while placing a pin.


Text Command (Symbol Editor Draw Menu)

Adds a text string.  Enter the text string in the dialog.  Move the text into position with the cursor, and click to place the text.  You can edit the size of the text by double-clicking on the desired text.  When the Change Text dialog appears, enter the size of the new text (by percent) in the Size text box.  The default is 100%, so for example, if you want the text to be half of its original size, type 50 in the Size text box.


Bbox Command (Symbol Editor Draw Menu)

Resizes the bounding box that surrounds a symbol.  When you choose this item, the cursor changes to a pencil shape.  Click to begin sizing the bounding box.  All of the graphics and pins for the symbol must be contained within the bounding box.  Resize the box by selecting the location of the lower right corner of the box and click to place it.  The bounding box defines the selection area of the symbol when placed on a schematic.


Origin Command (Symbol Editor Draw Menu)

Changes the origin, or reference point for the part.  Typically, this will be at the connection point of the upper leftmost pin.  When you place a part, or substitute one part for another part, the part is placed according to its reference point.  The default reference point is shown by a small square on the part.  When you choose Origin, the cursor becomes a pencil-shape.  Move the pencil to the new location for the reference point, and double-click to fix the origin.


Repeat Command (Symbol Editor Draw Menu)

Repeats the last command performed.


New Command (Symbol Editor Part Menu)

Creates a new symbol.  Displays the Part Definition dialog which lets you select the type of symbol you are creating.

See Also:

Definition command (Symbol Editor Part Menu)


Copy Command (Symbol Editor Part Menu)

Copies an existing part from one of the Symbol Library files and makes it the current part.  In the dialog, enter the name of an existing part to copy and the new part name.  Choose items from the Edit menu to modify the graphics of the symbol, or to change its definition.


Get Command (Symbol Editor Part Menu)

Edits an existing symbol in the current library.  In the dialog, specify the name of the part, or select it from the list box.  Select Edit or double-click on the list item to bring up the part.

This part becomes the current part, and its name is displayed in the Symbol Editor title bar.  You can then choose items from the Edit, Graphics, or Parts menu in the Symbol Editor to edit the definition..


Remove Command (Symbol Editor Part Menu)

Delete a part(s) from the current Symbol Library file.  You can select an item from the list, or type in a name and click Delete, or double-click on the list item.  Select Cancel when finished.  Note:  When you click Delete, the selected symbol will be removed from the current Symbol Library file in memory.  The changes made are permanent when the library file is saved to disk.


Save To Library Command (Symbol Editor Part Menu)

Saves the current part to a library other than the current library.


Attributes Command (Symbol Editor Part Menu)

Defines new part attributes or modifies existing attributes.

Note:  Attribute names are not case-sensitive; the TEMPLATE attribute is the same as the template attribute.

When you choose Attributes, a dialog like the one below appears.

To add a new attribute to the list:

Type in the new name in the Name text box and its value in the Value text box, then click Save Attr.

To modify an existing attribute:

Select an attribute from the displayed list.  Once the attribute has been selected, the attribute Name/Value pair will appear in the respective edit controls.  If you would like to change the attribute name, enter a new name in the Name text box.  If you change only the Name, a new attribute will be added to the list when Save Attr is selected, and the old one will remain unchanged.  To edit the value, enter the changes in the Value text box.  Click on Save Attr when finished.  The attribute changes will be reflected in the list box.

To delete an attribute from the list:

Select the attribute and click Del Attr.  The attribute Name/Value pair will be removed from the list.

If you specify that an attribute Name/Value pair is to be displayed on the schematic, they will be displayed when the main Symbol Editor window reappears.  To change the location of their display (which will default to the upper left corner of the symbol), select the attribute text and drag it to the desired location.

Name
Specifies the attribute name (i.e., PART, REFDES, and TEMPLATE).  If the Name you enter is the same as that of an existing attribute name in the list, the old attribute Name/Value pair will be overwritten with the new attribute value when modified.

Attribute names can use only alphanumeric characters.

Value
Specifies the attribute value.

Changeable in schematic
Specifies whether the attribute value can be changed on an instance by instance basis n the Schematic Editor.

Keep relative rotation
When enabled, causes the attribute to be rotated along with the part if the part is rotated on a schematic.

What to Display
Specify the combination of attribute name and value text, if any, that is to be made visible on the schematic.

Display Layer
Defines the layer upon which the attribute name and/or value will be displayed.  Whether a layer is displayed and/or printed can be configured using the Options/Set Display Level command.


Definition Command (Symbol Editor Part Menu)

Edits the part description, or add a new part description.

Dialog Box Options

Description
Defines the textual description of the symbol.  This description is displayed in the Schematic Editor when the Draw/Get New Part/Browse command is chosen.

Part Name
Specifies the most commonly used full name of the part.  This name, or an alias, is the name that will be used to create netlists and to bring an instance of the part into the schematic.  If Part Name has not been specified at the time you save this part, you will be prompted for the part name.

Alias List
Provides the exact electrical equivalents of the part that can be used to reference the symbol.

AKO Name
(stands for A Kind Of); if a symbol contains an AKO Name, it means that it will use the graphics, pins, and attributes of the named part (the AKO base part).  Attributes on the current symbol will override those from the AKO, and new attributes may be added.  For symbols having an AKO specified, the symbol it refers to must reside in the same Symbol Library file.  On symbols having an AKO, you can only edit the attributes and the description, you cannot edit the graphics, pins, or template.

Type
Defines the type of the symbol being edited.  Symbol types are:

component	electrical part or hierarchical symbol

annotation	non-electrical symbol

hier port	Interface port,  Connects between levels of hierarchy.

global port	connects between schematics

offpage port	connects between pages of a schematic

titleblock	page title block

border	page border

marker	Probe marker placed using one of the Marker menu commands

viewpoint	displays the bias point voltage of the net to which it is connected

current probe	displays the bias point current

optimizer parameter

PSpice Optimizer setup for each design parameter to be optimized

stimulus	simulation input waveforms set up using the Stimulus Editor

simulation control

symbols corresponding to PSpice and PLogic dot commands used in netlists 	(e.g., .IC, .NODESET)

Add
Adds alias part names to the alias list.  Simply type in the alias names of the electrically equivalent parts, and click Add to add each one to the list.

Delete
Removes the selected alias from the list.


Pin List Command (Symbol Editor Part Menu)

Displays the list of all pins for the current symbol.  If the symbol is a non-AKO symbol, you can edit the pin information.

To modify a pin:

Select a pin from the list appearing in the upper right corner of the dialog.  The values for that pin will appear in the edit controls.  Once you have entered the desired values, click OK Pin and the modified pin attributes will be reflected in the list.

Pin Name
Pin identifier.  It can also be used to define the number of signals that must be contained in a connecting wire or bus.

Pin names cannot use the following characters: , ( ) { } | & ~ ^ ;

Type
Determines how the pin will be displayed on the schematic.  The default is normal, which is a 10-unit line segment.

Display Name
When enabled, specifies that the name of the attribute is to be visible on the schematic.

Hidden
Sets a pin to be invisible in the Schematic Editor.  Note that hidden pins cannot be wired up in the Schematic Editor.  Use the Net text box to specify connectivity.  You can change the value of the IPIN attribute for this pin in the Schematic Editor to modify its connectivity.

Net
Specifies the default name of the net to which a hidden pin will be connected in the Schematic Editor.

Modeled Pin
Indicates that this is a modeled pin.  If the pin is not part of the simulation model (such as balance and offset pins on some opamps) then the box should be unchecked.  When the box is unchecked, the pin is marked as not simulated and a FLOAT=u attribute is applied to the pin.  This allows the netlister to pay special attention to the pin of there are fewer than two connections at its node.  If that is the case, a resistor to ground is added for simulation.

If the Modeled Pin checkbox is not marked, the Float list box (below) is disabled.

Float
Provides a list box that allows you to select a default action that the netlister will take if the pin is unconnected.  The choices are as follows:

RtoGND	add a large resistor to ground for the pin

UniqueNet	generate a unique node to monitor with a Probe marker

Error	cause netlister to fail and generate Unconnected Pin error

OK list
Select this when you are done making changes to the pin list.

Edit Attributes
Displays the  Attributes dialog letting you change the pins attributes.  This dialog lets you change whether or not pin numbers are displayed for the symbol.


Get Symbol Graphics Command (Symbol Editor Part Menu)

Imports the graphics from an existing symbol onto the current symbol.  Only the graphics portion of a symbol is imported.  In the dialog, specify the part name for the symbol to be imported by typing in the name directly, or selecting from the list.  You may use this command with any type of symbol.

Dialog Box Options

Select Library
Specifies a symbol library other than the current library from which to get the graphics.


Export Command (Symbol Editor Part Menu)

Writes the part definitions chosen from the list of parts in the current Symbol Library file, to a text file and gives the exported file a ".sym" extension if no extension is specified.  This command allows you to transfer symbols from one library file to another, or from one platform to another.  It allows you to manipulate individual symbols as files, if desired.


Import Command (Symbol Editor Part Menu)

Reads the text file assuming a ".sym" extension (if none is specified) and makes it the current part; it can then be saved to the current Symbol Library file.


New Command (Symbol Editor Packaging Menu)

Creates a new package definition.

Dialog Box Options

Package Name
Name of the package definition.

AKO
Displays the name of the package definition or base definition.  If no AKO is displayed, no base definition is being used.

# of Gates
The number of gates per package.  The default is one.

# of Gate Types
The number of different gate types defined for the package.  The default is one.

Note:  It is unusual to have more than one gate type in a package; some ECL parts are the most notable exceptions.

Package Types
List of package types (footprints) available for the device.  The pin assignment list for the currently selected package type is shown.  If the entry is a comma-separated list of package types, then they all have the same pinout or set of pin assignments.  To see the pin assignments for other package types, select another entry from the list.

Change AKO
Displays a dialog to allow you to enter the name of another package definition that is A Kind Of (base definition).  If a definition is an AKO, it shares the gate, package, and pin number information of the base definition.

Edit Gate Types
Edit the list of gate types defined for the package.

Edit Package Types
Modifies the list of package types (footprints)  from the Package Types list.

To add a package type:

Enter the name or select from the Configured Package Types drop-down list, then click Add.  Each entry in the list represents a different pin-assignment list.  An entry can consist of a single package type or a comma separated list of package types.

To delete a package type:

Select a type from the current list of package types, then click Delete.

Pin Assignments
Displays the list of the pin names and their pin numbers for each gate for the currently selected package and gate type.  Entries are of the form:

<pin name>=<pin number>,<pin number>

with the pin numbers in the same order as the gates.

To modify the pin assignments list:

Click Edit Pins.   The shared pins and pin swap lists can also be modified by choosing Edit Shared Pins and Edit Pin Swaps, respectively.

Gates
Displays the list of gates used by the currently selected gate type.

Gate Type
Displays the gate type name whose pin assignments are currently shown.  To view the pin assignments for another gate type, select an entry from the drop-down list.

Shared Pins
Lists the names and numbers of pins shared by the gates within the package (for the currently selected package types).

Pin Swaps
Lists the swappable pins for the current gate type.

Edit Pins
Displays the Edit Pin Assignment dialog which lets you modify the pin number assignments for the currently selected pin out.

Dialog Box Options

Package Types
Identifies the current package type or comma-separated list of package types for which the pin assignments are valid.

Gate
Must be one of the defined gates for the current gate type.

Pin Name
Must be the same name used on the symbol.

Pin No.
The alphanumeric pin number which can be modified.

If there is a list of pins in the list box, you can automatically step through the list for editing as follows:

1.	Click on the first entry.

2.	Modify the pin number in the Pin No. text box.

3.	Choose Save Assignment or press <Enter>.  The next pin number is automatically displayed in the edit controls.

To remove pins that do not belong in the list for the current gate type, choose Delete.  These are typically the shared pins in a multi-gate package.

Edit Shared Pins
Edits the list of pins shared by all gates  The dialog is similar to that for Edit Pins.

Edit Pin Swaps
Edits the list of swappable pins for the current gate type.

To define swappable pin assignments:

1.	Select two or more entries in the Pin Names list box.

2.	Choose Assign.

To remove all pin swap assignments from the Pin Swaps list:

1.	Choose Clear.

Dialog Box Options

Package
Name of the package definition being edited.

Gates
Lists the set of gates corresponding to one of the gate types in the current package.

Pin Names
Multiple-select list box from which you can choose equivalent or swappable pins.

Pin Swaps
List of the current pin swap assignments.  Each entry in the list is a comma-separated list of the pins within a gate (each identified by pin name) that can be swapped with one another.

Print
Prints a hard copy of the package definition information.  (Select the printer  through the File/Printer Select command.)


Copy Command (Symbol Editor Packaging Menu)

Create a new package definition from an existing one.  As with Part/Copy the definition may be copied from the current library file or a different library file.


Get Command (Symbol Editor Packaging Menu)

Edit any package definition in the current Package Library file.


Remove Command (Symbol Editor Packaging Menu)

Deletes package definition(s) from the current library file.  A list of the package definitions for the current library file are shown.  You may delete one or more of the definitions.  You can select an item from the list, or type in a name and click  Delete, or double-click on the list item.  Select Cancel when finished.


Edit Command (Symbol Editor Packaging Menu)

Edits the package information for the current symbol.  Only the Package Library file with the same name as the current Symbol Library file is searched.  If there is no package definition, you will be asked if you wish to create one from the symbol's pin information.  The Package Definition dialog will be shown with values for the current symbol automatically added.

Note:  If you were first  prompted with Use symbol information to create default pin assignments?, and replied Yes, the package type named in the Package Types text box is `?'.  To change this, choose the Edit Package Types button; see the New command in the Packaging Menu for an explanation of the Edit Package Types dialog.   To be sure that all of the pin assignment information established for the current symbol is not lost, do not delete the `?' entry.  Instead, rename this entry as follows:

1.	Select the `?' entry in the list box.

2.	Update the package type name in the Packages Type(s) per Pin Assignment text box.

3.	Choose Change.


Configure Package Types Command (Symbol Editor Packaging Menu)

Edits the list of package types and the classes to which they belong.  This list is used by the packager in the Schematic Editor to determine which package type to assign when there are multiple package types available for a part.


Export Command (Symbol Editor Packaging Menu)

Writes one or more package definitions to an ASCII text file with a ".pkg" extension (if none is specified).


Import Command (Symbol Editor Packaging Menu)

Read one or more package definitions from an ASCII text file.


Fit Command (Symbol Editor View Menu)

Sets the viewing scale to show all graphics components (including those which lie outside the symbol's bounding box) within the viewing window.  The actual fit percent (that is, the measure of how closely the window fits the contents) is configured through the VIEWFITPERCENT setting in the "msim.ini" file. (Refer to the Installation Guide for specifics.)


In Command (Symbol Editor View Menu)

Changes the viewing scale to view your schematic at a closer range, so that items appear larger.  Use the cross hair to select the center of the viewing area.  Each In command zooms the display approximately 20%.


Out Command (Symbol Editor View Menu)

Changes the viewing scale so that you can see a larger area of your symbol.  Click to define the center of the viewing area.  Each time you subsequently double-click right, the viewing scale decreases by about 30%.


Area Command (Symbol Editor View Menu)

Changes the viewing scale to show the selected area.


Previous Command (Symbol Editor View Menu)

Restores the viewing scale and area shown to what they were previously.


Entire Symbol Command (Symbol Editor View Menu)

Displays the entire symbol at once.


Redraw Command (Symbol Editor View Menu)

Redraws (refreshes) your screen display.


Pan New Center command (Symbol Editor View Menu)
Pan - New Center Command (Symbol Editor View Menu)

Retains the current zoom scale and pans the symbol display so that the point selected is centered in the display.


Display Options Command (Symbol Editor Options Menu)

Set up your screen display as desired.  The various options which can be toggled on or off are explained below.

Dialog Box Options

Grid On
Turns the grid display on or off.

Snap to Grid
Causes components to snap to the nearest grid point when you place them; before placing, objects may be moved freely.  If Snap to Grid is disabled, movement is by grid units.

Stay on Grid
Places components strictly on the grid.  Components always stay on the grid lines, even while being moved.

Status Line
Turns the status line at the bottom of your screen on or off.

Cursor X and Y
Turns the X and Y coordinates display (shown on the status line) on or off.

Grid Spacing
Defines the horizontal and vertical grid spacing on your drawing area.  The default spacing is 10 units.  This corresponds to (and is displayed as) .10 inches or 2.5 millimeters depending on the page size selected in the Schematic Editor (US-Standard or metric).  The Symbol Editor grid spacing is independent of the Schematic Editor grid spacing.  The minimum grid spacing allowed is 0.01 (US).

Gravity
Specifies the distance between the cursor and an object on the schematic, in order to select it.  The default is  3 units (.03 inches or .75mm).  When manipulating larger objects, it is advisable to set the gravity to a higher number.

Text Stay on Grid
Keep text on text grid lines.

Toolbar
Turns on and off the display of the toolbar.

Spacing
Defines the grid spacing for text separately from the graphics grid spacing.


Auto-Repeat Command (Symbol Editor Options Menu)

When enabled, automatically duplicates an object at a specified distance when the repeat function (double-click right) is used.  For example, you can use Auto-Repeat with the Pin command to repeatedly place part pins.  Each repeated pin being placed is offset from the one placed before it.  On the PC, you can also use the <Space Bar> to repeat the previous command.

Dialog Box Options

Enable Auto-Repeat
Turns Auto-Repeat on or off.  Off is the default setting.

Horizontal and Vertical Offsets
Defines the distance in which objects are automatically placed in relation to the previously placed instance of the object.


Set Display Level Command (Symbol Editor Options Menu)

Sets whether to have the text or specific components displayed on the screen, on the hard copy, or on both.  The default is to display them both on the screen and on the hard copy.

Select Printer to print the text, or Screen to display the text on the screen.  You may choose both Printer and Screen at the same time.  You may also choose as many text types as you wish to be displayed from the choices presented.   Clear All will clear any choices that have been set.  Set All will set all choices to be displayed on the screen and printed on the hard copy.


New Schematic Window Command (Symbol Editor Window Menu)

Creates a new window for schematic design and returns you to the Schematic Editor.


Close Command (Symbol Editor Window Menu)

Closes the current Symbol Editor window.  If you have made changes you will be prompted to save changes before closing.


Arrange Command (Symbol Editor Window Menu)

Displays a dialog which allows you to select an arrangement for all

of the open windows.