Product Documentation
OrCAD Capture Reference Guide
Product Version 17.4-2020, June 2020

Property Sheet Pane

This pane contains the following sections related to part and pins:

In an existing part, depending upon the object selected, the required section in the property pane opens.

This pane has the following functions:

Package Properties

To open this section in the Property Sheet pane

When you select a part in the part editor, and related package properties appear in the Package Properties section of the Property Sheet pane.

Use this control... To do this...

Part Numbering

Displays the numbering format (Alphabetic or Numeric) that is added as suffix to the current part reference for the new or selected part.

If Alphabetic is selected, you can create a maximum of 26 sections.

If Numeric is selected, you can create a maximum of 1024 sections.

This field has a drop-down list using which you can change the part numbering format after part creation or during part editing.

Package Type

Displays whether all the parts in the package have the same graphical representation (homogeneous) or different graphical representations (heterogeneous).

The package type can only be set at creation time. This option is not available when you edit the part later.

You should not cut and paste parts between homogeneous and heterogeneous packages.

PCB Footprint

Specify the PCB Footprint name to be included for this part in the netlist. Contains a value for a device consisting of zero or more pads, other objects, and a name.

PCB Footprint is a reserved property name. If you want to make its value visible on the schematic page, you must do so in the property editor.

Part Reference Prefix

Specify the part reference prefix, such as C for capacitor or R for resistor.

Section Count

Specify the number of parts in the package. The Section Count field shows the count specified in the Parts per Pkg or No. of Sections field during part creation.

If Alphabetic is selected in Part Numbering (while part creation), section names will start with A.

If you create a single-section part with Alphabetic numbering, section name is not displayed and it is automatically converted into a part with Numeric numbering.

If Numeric is selected in Part Numbering (while part creation), section names will start with 1.

You can modify the number of sections after part creation.

Part Aliases

Click the Update button to open the Update Alias dialog box, which is used to add and edit part aliases.

Part Properties

To open this section in the Property Sheet pane

Open or select a part in the part editor, and the related part properties appear in the Part Properties section of the Property Sheet pane.

Use this control... To do this...

Name

Displays both the name and normal or convert view of the part. The part name appears to the left of the period, and the view appears to the right. This property is read-only.

suffix

Is used to indicate if the view is Normal or Convert for the current section of the part. This is a read-only property.

Implementation Path

Specify the filename and directory to the child schematic.

Click icon to browse the location of the child schematic.

Implementation

Specify the name of the child schematic for the part.

Implementation Type

Specify the implementation type. For information about various implementation types, see Attach Implementation dialog box.

Value

Specify the part value. If this is not specified when you place the part in a schematic folder, Capture uses the part name.

Pin Name Visible

Select this option to specify if the pin names are visible in the schematic page editor and part editor.

Pin Number Visible

Select this option to specify if the pin numbers are visible in the schematic page editor and part editor.

Pin Name Rotate

Select this option to specify if the pin names and pin numbers rotate with top and bottom pins.

Click this icon to add user-defined properties.

You can add any user-defined properties in this section. Some of the commonly used properties are available in the drop-down list.

You can also delete an existing user-defined property. Click the Delete icon ( ) next to any user-defined part property to delete it.

Any user property added to the current section of the part is applied to all sections.

Pin Properties

To open this section in the Property Sheet pane

Select a pin in the part editor, and the properties related to the pin appear in the Pin Properties section of the Property Sheet pane.

Use this control... To do this...

Name

Specify the pin name. You can create a pin name with an overbar by adding a backslash (\) after every letter in the pin name.

Number

Specify the pin number. The pin number does not need to be a number; it can be alphabetic. If it ends in a number, it is incremented by one after each pin is placed.

The pin number has a limit of 32 characters. Characters that exceeds this limit will be truncated.

Shape

Select the pin shape from the list of pin shapes.

Type

Select the pin type from the list of pin types.

Pin Visible

Specify the pin visibility on the schematic page. Only power pins can be set to not visible.

Order

Specify the order in which pin is placed in a part. This is a read-only property.

User Properties

Click the add icon, in this section to add a user-defined property.

You can also delete an existing user-defined property. Click the Delete icon ( ) next to any user-defined pin property to delete it.

Any pin property added to the current section of a homogeneous part is applied to all sections in the same view (Normal or Convert).

For a heterogeneous part, pin properties are not copied to other sections.
Bus pins cannot be used directly as netlisting pins. Their main purpose is to make it possible to use nonprimitive parts more easily by connecting large numbers of signals to a child schematic folder.
You can place one pin on a part that represents all pins for a bus. Such a pin is called a bus pin. Bus pins use the same naming convention as buses.

Text Properties

To open this section in the Property Sheet pane

Select a comment text in the part editor, and related text properties appear in the Text Properties section of the Property Sheet pane.

Use this control... To do this...

Text

Displays the text.

Font

Displays the current font style and also allows you to change it from the drop-down list.

Font Size

Displays the current font size and also allows you to change it from the drop-down list.

Bold

Select this check box to modify the text format.

Italic

Select this check box to modify the text format.

Justification

Specify the text justification for the comment text as Default, Left, Center, or Right.

Basic Attributes

To open this section in the Property Sheet pane

Select any object in the part editor. All properties related to the object (text, graphical, or position-related) appear in this section. Some of the properties are listed in the following table:

Use this control... To do this...

<Object Name>

Displays the value of the selected object.

Rotation

Displays the rotation of the selected object.

Location

Displays the X and Y coordinates of the selected object on the canvas.

Font

Displays the current font style of the selected object. You can also change the font style from the drop down list.

Color

Displays the color of the selected object and also allows you to change it from the drop-down list.

Font Size

Displays the current font size. You can also change the font size from the drop down list.

Bold

Select this check box to make the object value bold.

Italic

Select this check box to italicize the object value.

Justification

Specify the justification for the object value as Default, Left, Center, or Right.

Display Properties

Click the Display Property icon ( ) next to any part property to specify the visibility for the property name and value. It allows you to set the display option of the selected property and its value, such as Do Not Display, Value Only, and Name Only.

Delete Current Section

Click the Delete Current Section button to delete the current section of the part.

This button is disabled for a part with a single section and for a heterogeneous part with only two sections.

To select any specific section of a heterogeneous part, click the drop-down at the left bottom corner of the canvas.

Add Convert View

Click the Add Convert View button to specify the convert view for a part.

Delete Convert View

Click the Delete Convert View button to delete the convert view for a part.

Edit Pins

To open this dialog box, do any one of the following:

This dialog box enables you to view pin information according to pin selection. You can view pin information for:

Operations in the Edit Pins dialog box

This table lists the various operations you can perform in the Edit Pins dialog box.

Operation

Function

Press F2

Edit the current cell.

Press Tab

Shift to the next cell across the row.

Press SHIFT+Tab

Shift to the next cell across the row in the reverse direction.

Press Enter

Apply changes to the current cell and shift to the next row.

Press CTRL+C and CTRL+V
  • Copy and paste data in the same table.
    Or
  • Copy and paste data from Microsoft Excel.

In the edit pins table:

  • Pasting data from one cell into multiple cells copies the data to all the target cells.
  • Pasting data from many cells to multiple cells populates data only from the copied cells.

Drag the plus sign that appears at the bottom-right corner of a cell to copy its contents into multiple cells.

Use the range extender to populate other cells of a column with the same value.

Select a check box to display a column.

Clear the check box to hide a column.

Select the required column header check boxes above the edit pins table to show or hide the required columns.

Selection of the check boxes is maintained within a session of the part editor.

Double-click a column header.

Sort column data in ascending or descending order.

Operations between Part Editor Canvas and Edit Pins Dialog Box

The following table lists the various operations you can perform between the canvas and the Edit Pins dialog box.

Operation

Description

Select the required pins on canvas and open the Edit Pins dialog box.

Only the selected pins and their corresponding information is displayed in the table.

The size of the Edit Pins dialog box gets adjusted according to the number of pins selected.

Select all the pins on the canvas and open the Edit Pins dialog box.

Pin information of all the pins of the current section is displayed.

If you do not select any pin and open the Edit Pins dialog box.

All the pins for all the sections appear in the table.

Paste Options dialog box

To open this dialog box

  1. Ensure that the setting Enable the Paste Options mode is selected in the Extended Preferences Setup window.
  2. Select any number of pins.
    or
    Select any graphical object with any number of pins selected along with it.
  3. Copy the selection.
  4. Select Edit – Paste, press CTRL+V, or right-click and select Paste.
    If you copy only pins, the Paste Options dialog box opens immediately.
    If you copy any graphical object along with the pins, the Paste Options dialog box opens after you place the copied graphical object(s).
    The pin location of the copied part is retained only if the destination part has no pins else the copied pins are pasted as a pin array.
  5. Modify the pin information from the required section.
  6. Click the Paste button.
  7. Click to place the pin at the required location.

Part Aliases dialog box

To open this dialog box

Click the Part Aliases button in the New Part Properties dialog box.

Use this control... To do this...

Alias Names

Select an alias name from the displayed list.

New

Open the New Alias dialog box to add new aliases.

Delete

Delete the selected alias from the list.

Part Search dialog box

To open this dialog

Click Part Search in the Place Part dialog box.

Use this control... To do this...

Part Name

Specify the part name to search for. Use an asterisk (*) to match any string of characters, and a question mark (?) to match any single character.

Libraries

Displays the location of all libraries for the part specified in Part Name. After Capture has searched for the part and located it, select the part from one of the libraries and click OK. If the library is configured in the Place Part dialog box, then Capture closes this dialog box, and selects the part in the Place Part dialog box.

Library Path

Specify the path containing libraries for Capture to search through. Set this to your library directory.

Begin Search

Begin searching for the part specified by Part Name, and in the directory specified by Library Path.

Browse

Display a standard Windows dialog box for selecting files.

Place Bookmark dialog box

To open this dialog

In the schematic page editor, choose Bookmark (see Bookmark command)from the Place menu.

Use this control... To do this...

Name

Specifies the bookmark's name.

Place Ground dialog box

To open this dialog

In the schematic page editor

Choose Ground (see Ground command) from the Place menu.

OR

Click the Ground button on the Draw Electrical toolbar.

Use this control... To do this...

Symbol

Specify a symbol to select and view. Use an asterisk (*) to match any string of characters, and a question mark (?) to match any single character.

Symbol List

Displays a list of power symbols and ground symbols in the libraries selected in the Libraries list box that match what's entered in the Symbol text box. When you select an object in this list, its name appears in the Symbol text box, and its graphic appears in the preview box. Select an object from the list of symbols available in the selected libraries.

Libraries

Select one or more libraries from the list of available libraries. The symbol list displays the objects from the selected libraries. You also select libraries from the Libraries list box to remove them from the list.

The CAPSYM.OLB, which is the default library in Capture now includes the PSpice ground (0) symbol. Use the ‘0’ symbol to place a PSpice ground 0 symbol in your design. If your design does not have a PSpice ground (0) symbol, then the PSpice analog simulation may not run. To place a PSpice ground ‘0’ symbol in your design, see Placing PSpice ground 0 symbols for PSpice simulations.

Preview box

Displays the graphic of the selected object.

Name

Specify the object's name.

Add Library

Display a standard Windows Open dialog box for adding a library to the Libraries list box. You can add a library in SDT format. If you do, you can save the library in the Capture format (.OLB).

Remove Library

Remove the selected library or libraries from the libraries list box.

Place NetGroup dialog box

The NetGroup dialog displays when you choose NetGroup from the Place menu.

Use this control... To do this...

Add NetGroup

Click this button to open the New NetGroup dialog to create a NetGroup.

Modify NetGroup

Click this button to open the Modify NetGroup dialog to modify a NetGroup.

You need to click the check mark next to a NetGroup name to open the associated NetGroup definition in this dialog.

Delete NetGroup

Click this button to delete selected NetGroups.

Import NetGroups

Click this button to import NetGroups definition Xml files.

Instance Name

Enter the instance name of a named NetGroup to place on the schematic page.

Place NetGroup Block

Check this box to place the NetGroup as a block on the schematic page.

Place Unnamed NetGroup

Check this box to place the NetGroup as an unnamed NetGroup block on the schematic page.

Place Off-Page Connector dialog box

To open this dialog

In the schematic page editor

Choose Off-Page Connector (see Off-Page Connector command) from the Place menu.

OR

Click the Off-Page Connector button on the Draw toolbar.

Use this control... To do this...

Symbol

Specify a symbol to select and view. Use an asterisk (*) to match any string of characters, and a question mark (?) to match any single character.

Symbol List

Displays a list of off-page connectors in the libraries selected in the Libraries list box that match what's entered in the Symbol text box. When you select an object in this list, its name appears in the Symbol text box, and its graphic appears in the preview box. Select an object from the list of symbols available in the selected libraries.

Libraries

Select one or more libraries from the list of available libraries. The symbol list displays the objects from the selected libraries. You also select libraries from the Libraries list box to remove them from the list.

Preview box

Displays the graphic of the selected object.

Name

Specify the object's name.

Add Library

Display a standard Windows Open dialog box for adding a library to the Libraries list box. You can add a library in SDT format. If you do, you can save the library in the Capture format (.OLB).

Remove Library

Remove the selected library or libraries from the libraries list box.

NetGroup OffPage

Place the off-page connector as a named NetGroup off-page connector.

Select the NetGroup, to be used, from the drop-down list of NetGroups.

Show UnNamed NetGroup

Place the off-page connector as an unnamed NetGroup off-page connector.

Place Hierarchical Block dialog box

To open this dialog

In the schematic page editor

Choose Hierarchical Block (see Hierarchical Block command) from the Place menu.

OR

Click the Hierarchical Block button on the Draw toolbar.

Use this control... To do this...

Reference

Specify the hierarchical block's name.

Primitive

Default

Use the default primitive setting, which for hierarchical blocks is nonprimitive. The default setting for hierarchical blocks is set in the Hierarchy tab of the Design Template dialog box (see Design Template command).

Yes

Indicate the hierarchical block is a primitive.

No

Indicate the hierarchical block is nonprimitive and descends in hierarchy.

User Properties

Display the User Properties dialog box so you can modify the hierarchical block's user defined properties.

Implementation

Implementation Type

Schematic View Indicate that the attached implementation is a schematic folder. Capture automatically generates the appropriate hierarchical pins for the block based on the hierarchical ports.

VHDL Indicate that the attached implementation is a VHDL entity. Capture automatically generates the appropriate hierarchical pins for the hierarchical block based on the port declarations in the VHDL entity.

EDIF Indicate that the attached implementation is an EDIF netlist. If your design includes EDIF implementations for hierarchical blocks, you must specify the hierarchical pins for the block; Capture will not generate them from the EDIF netlist. Also, if your design includes EDIF implementations, you can simulate them, but you cannot compile or build them.

Project Indicate that the attached implementation is a Capture programmable logic project. You must specify the hierarchical pins for the hierarchical block; Capture will not generate them.

PSpice Model Indicate that the attached implementation is a PSpice model file. You must specify the hierarchical pins for the block; Capture will not generate them.

PSpice Stimulus Indicate that the attached implementation is PSpice stimulus file. You must place the hierarchical pins on the block. Capture will not generate them.

Verilog Indicate that the attached implementation is a Verilog model. Capture automatically generates the appropriate hierarchical pins for the hierarchical block based the Verilog model.

Attaching an implementation does not automatically add that file, project, or schematic folder to the project. You must specifically add the implementation to the project with the Project command (Edit menu).

Implementation name

Specify the name of the attached schematic folder, VHDL entity, netlist, or project for the hierarchical block.

Path and filename

Specify the path and filename for the library of the attached object. Use the Browse button to locate the file, or supply both the path and filename. If the attached object is in the same design as the hierarchical block you are placing, leave this option unspecified.
If you attach external schematic folders or other files to hierarchical blocks in a design or parts in a library, be sure to include the attachments when you pass the design or library to a board fabrication house or to another engineer. Attached schematic folder and other files are not carried along automatically when you copy or move a part, schematic folder, or schematic page to another library, design, or schematic folder. Only the "pointers" to the attached schematic folder and files—that is, their names and the names of the designs or libraries that contain them—are carried along. Attached files work much like their counterparts in email—they do not provide an alternative definition of the part (as do attached schematic folders).
Be careful not to create recursion in your design. Capture cannot prevent recursion, and the Design Rules Check command does not report it. Recursion causes Capture to process infinitely as it tries to expand the design, resulting in the loss of any changes you've made to your design since it was last saved.
When you attach a schematic folder to a part or hierarchical block, you can specify a full path and filename in the Library text box. So, although you can specify a library that hasn't been saved, you should not try to descend into the attached schematic folder until the library that contains the schematic folder has been saved. If you don't specify a full path and filename in the Library text box, Capture expects to find the attached schematic folder in the same design as the part of hierarchical block to which it is attached. If the specified schematic folder doesn't exist in either the design or library, Capture creates the schematic folder when you descend hierarchy on the part or the hierarchical block. For compatibility with future versions of Windows, Capture preserves the case of the path and filename as you specify them in the Library text box.
Once you have attached a file and associated a text editor with it, you can use the Descend Hierarchy command to open that file. If you have an attached schematic folder as well as an attached file, Descend Hierarchy opens the schematic folder and not the file.

Place Hierarchical Pin dialog box

To open this dialog

In the schematic page editor

Choose Hierarchical Pin (see Hierarchical Pin command) from the Place menu.

OR

Click the Hierarchical Pin button on the Draw toolbar.

Use this control... To do this...

Name

Specify the hierarchical pin's name.

Type

Select the pin type from the list of pin types.

Width

Specify if the pin connects to a bus or a wire. If bus is specified, the hierarchical pin must connect to a bus; otherwise, it must connect to a wire.

User Properties

Display the User Properties dialog box so you can edit the pin's properties.
Bus pins cannot be used directly as netlisting pins. Their main purpose is to make it possible to use nonprimitive parts more easily by connecting large numbers of signals to a child schematic folder.
You can place one pin on a part that represents all pins for a bus. Such a pin is called a bus pin. Bus pins use the same naming convention as buses.
You can use bus pins in most cases where you can use scalar pins. For example:

Place Hierarchical Port dialog box

To open this dialog

In the schematic page editor

Choose Hierarchical Port (see Hierarchical Port command) from the Place menu.

OR

Click the Hierarchical Port button on the Draw toolbar.

Use this control... To do this...

Symbol

Specify a symbol to select and view. Use an asterisk (*) to match any string of characters, and a question mark (?) to match any single character.

Symbol List

Displays a list of hierarchical ports in the libraries selected in the Libraries list box that match what's entered in the Symbol text box. When you select an object in this list, its name appears in the Symbol text box, and its graphic appears in the preview box. Select an object from the list of symbols available in the selected libraries.

Libraries

Select one or more libraries from the list of available libraries. The symbol list displays the objects from the selected libraries. You also select libraries from the Libraries list box to remove them from the list.

Preview box

Displays the graphic of the selected object.

Name

Specify the object's name.

Add Library

Display a standard Windows Open dialog box for adding a library to the Libraries list box. You can add a library in SDT format. If you do, you can save the library in the Capture format (.OLB).

Remove Library

Remove the selected library or libraries from the libraries list box.

NetGroup Port

Place the hierarchical port as a named NetGroup port.

Select the NetGroup, to be used, from the drop-down list of NetGroups.

Show UnNamed NetGroup

Place the hierarchical port as an unnamed NetGroup port.

Place IEEE Symbol dialog box

To open this dialog

In the part editor, do one of the following:

Place Net Alias dialog box

To open this dialog

In the schematic page editor

Choose Net Alias (see Net Alias command) from the Place menu.

OR

Choose the Place net alias button on the Draw toolbar.

OR

Press the N key.

Use this control... To do this...

Alias

Enter the net alias name in the text box.

Color

Specify the color of the net alias.

Rotation

Specify the rotation of the net alias or text.

Font

Change

Display the Font dialog box so you can select a font.

Use Default

Change the font to the default font specified in the Design Template dialog box.

NetGroup

NetGroup Aware Aliases

Select to assign a NetGroup to a bus. Select an existing NetGroup from the list or edit to add a new NetGroup. The width of the alias is the same as the specified NetGroup.

Click the Off-Page Connector button on the Draw toolbar.

Use this control... To do this...

Symbol

Specify a symbol to select and view. Use an asterisk (*) to match any string of characters, and a question mark (?) to match any single character.

Symbol List

Displays a list of off-page connectors in the libraries selected in the Libraries list box that match what's entered in the Symbol text box. When you select an object in this list, its name appears in the Symbol text box, and its graphic appears in the preview box. Select an object from the list of symbols available in the selected libraries.

Libraries

Select one or more libraries from the list of available libraries. The symbol list displays the objects from the selected libraries. You also select libraries from the Libraries list box to remove them from the list.

Preview box

Displays the graphic of the selected object.

Name

Specify the object's name.

Add Library

Display a standard Windows Open dialog box for adding a library to the Libraries list box. You can add a library in SDT format. If you do, you can save the library in the Capture format (.OLB).

Remove Library

Remove the selected library or libraries from the libraries list box.

NetGroup Port

Place the off-page connector as a named NetGroup off-page connector.

Select the NetGroup, to be used, from the drop-down list of NetGroups.

Show UnNamed NetGroup

Place the off-page connector as an unnamed NetGroup off-page connector.

Place Part dialog box

To open this dialog

In the schematic page editor

Choose Part (see Part command) from the Place menu.

OR

Click the Part button on the Draw toolbar.

Place Part Pane

Use this control... To do this...

Part

Specify the name of the part. Use an asterisk (*) to match any string of characters, and a question mark (?) to match any single character.

Part List

Displays a list of parts in the libraries selected in the Libraries list box that match what's entered in the Part text box. When you select a part in this list, its name appears in the Part text box, and its graphic appears in the preview box. Select a part from the list of parts available in the selected libraries.

You can filter the part list, using the Filter button described below.

Filter

Display the Specify Part Filter dialog box that allows you to restrict part searches in part libraries based on specific criteria.

For example, if you are a PSpice user, you can restrict your part library search such that only parts with associated PSpice simulation models will be listed in the Part List.

Libraries

Select one or more libraries from the list of available libraries. The part list displays the parts from the selected libraries. You also select libraries from the Libraries list box to remove them from the list.

Graphic

Select either Normal or Convert view. All parts have a normal view. Some parts have a convert view that can be used for things such as a DeMorgan equivalent part.

Add Library

Display a standard Windows Open dialog box for adding a library to the Libraries list box. You can add a library in SDT format. If you do, you can save the library in the Capture format (.OLB).

Remove Library

Remove the selected library or libraries from the libraries list box.

Reload Library Parts

Reloads the Capture library parts in the selected library.

As you reload the library parts, remember the following points:
  • To see the updated part, reselect library part in Place Part dialog. To update library with newly added or deleted parts, reload the library in Place Part dialog.
  • To enable the library parts update on selection, select the Refresh part on selection option in Preferences – Miscellaneous tab.

Packaging

Parts per Pkg

Displays the number of parts in the package.

Part

Select the part in the package to place on the schematic page.

Type

A package may be either homogeneous or heterogeneous.

Preview box

Displays the graphic of the selected part.

Application indicator

This feature uses icons to indicate whether the selected part has certain properties. The icon displayed for each property is described below. Note that, in the case of the Implementation Type property, only Implementation Type properties with values of “Schematic View” or “VHDL” are indicated with an icon.

Property: PCB Footprint. Value: Various values related to PCB layout.

Property: Implementation Type. Value: “Schematic View”

Property: Implementation Type. Value: “VHDL”

Property: Implementation Type. Value: “Verilog”

Property: PSpice Template. Value: PSpice syntax for part netlist entry

This icon is not associated with any property. It indicates that the part is associated with a template-based parameterized PSpice model.

Search Part

The Search for Part section of the Place Part dialog box is viewed if you click the Expand button.

Search For

Enter the part name (you can include wildcard characters) to search through the libraries for a specific part or parts.

Path

Enter the path of the library to search for the part. You can use the Browse button to select the library.

Libraries

Displays a list of libraries in which you searched for parts.

Add

Add libraries from the search library list to the Place Part library list.

Place Pin Array dialog box

To open this dialog

In the part editor, do one of the following:

Place Pin dialog box

To open this dialog

In the part editor, do one of the following:

Bus pins cannot be used directly as netlisting pins. Their main purpose is to make it possible to use nonprimitive parts more easily by connecting large numbers of signals to a child schematic folder.
You can place one pin on a part that represents all pins for a bus. Such a pin is called a bus pin. Bus pins use the same naming convention as buses.

You can use bus pins in most cases where you can use scalar pins. For example:

Do not use pins in the following situations:

Place Power dialog box

To open this dialog

In the schematic page editor

Choose Power (see Power command) from the Place menu.

OR

Click the Power button on the Draw toolbar.

OR

Press the F key.

Use this control... To do this...

Symbol

Specify a symbol to select and view. Use an asterisk (*) to match any string of characters, and a question mark (?) to match any single character.

Symbol List

Displays a list of power symbols and ground symbols in the libraries selected in the Libraries list box that match what's entered in the Symbol text box. When you select an object in this list, its name appears in the Symbol text box, and its graphic appears in the preview box. Select an object from the list of symbols available in the selected libraries.

Libraries

Select one or more libraries from the list of available libraries. The symbol list displays the objects from the selected libraries. You also select libraries from the Libraries list box to remove them from the list.

Preview box

Displays the graphic of the selected object.

Name

Specify the object's name.

Add Library

Display a standard Windows Open dialog box for adding a library to the Libraries list box. You can add a library in SDT format. If you do, you can save the library in the Capture format (.OLB).

Remove Library

Remove the selected library or libraries from the libraries list box.

Place Text dialog box

To open this dialog

In the schematic page editor, do one of the following:

Place Title Block dialog box

To open this dialog

In the schematic page editor

Choose Title Block (see Title Block command) from the Place menu.

OR

Click the Title Block button on the Draw toolbar.

Use this control... To do this...

Symbol

Specify a symbol to select and view. Use an asterisk (*) to match any string of characters, and a question mark (?) to match any single character.

Symbol List

Displays a list of title blocks in the libraries selected in the Libraries list box that match what's entered in the Symbol text box. When you select an object in this list, its name appears in the Symbol text box, and its graphic appears in the preview box. Select an object from the list of symbols available in the selected libraries.

Libraries

Select one or more libraries from the list of available libraries. The symbol list displays the objects from the selected libraries. You also select libraries from the Libraries list box to remove them from the list.

Preview box

Displays the graphic of the selected object.

Name

Specify the object's name.

Add Library

Display a standard Windows Open dialog box for adding a library to the Libraries list box. You can add a library in SDT format. If you do, you can save the library in the Capture format (.OLB).

Remove Library

Remove the selected library or libraries from the libraries list box.

Preferences dialog box

To open this dialog

In the schematic page editor or part editor, choose Preferences (see Preferences command) from the Options menu.

Use this tab... To do this...

Application Theme

Click the drop-down list to select the theme of the application.

Schematic Theme

Click the drop-down list to select the theme of the schematic page.

Colors/Print

Define the default color of objects such as aliases, wires, design variants, part not present, and pins. A standard Windows default Color dialog box appears when you click on the color of an item.

The check boxes next to the objects control whether the objects will be printed or plotted. If an object's box is selected, the object can be printed or plotted. Objects always appear on your screen, regardless of the setting of their check boxes.

The Use Defaults button resets colors to the default colors shipped with Capture.

The border and grid references of schematic pages use the color specified for title blocks.
Color specified in part editor for Pin Name, Pin Number, Part Properties, Part Reference Prefix, Part Value, and any user-defined property overrides the color selected in the Preferences dialog box.

Grid Display

Control the behavior and appearance of the grid display for both the schematic page editor and the part editor. See Grid Display tab for more information.

Pan And Zoom

Set auto scrolling options and zoom factor for both the schematic page editor and the part editor. See Pan and Zoom tab for more information.

Select

Specify selection options, change the maximum number of objects you can drag, and set tool palette visibility for both the schematic page editor and the part editor. For more information, see Select tab

Miscellaneous

Specify the fill style, line style, and line width for both the schematic page editor and the part editor. Also specify the line color for the schematic page editor. You can also define the session log font, set text rendering, set auto recovery intervals, and enable intertool communication. For more information, see Miscellaneous tab.

Text Editor

Specify font and color information for the text editor. Also specify tab setting in terms of character spacing, and highlighting options. For more information, see Text Editor tab.

Board Simulation

Specify the hardware development language to be used during board level simulation.

Color/Print tab

Use these options to specify the color settings for the different object types on a schematic page.

Use this control... To do this...

Basic colors

Shows the color of the object selected in the Colors tab.

To change the color, click the left mouse button on a different color and then click OK.

Custom colors

This feature is disabled in Capture.

Define Custom Colors

This feature is disabled in Capture.

Grid Display tab

Use these options to specify the appearance of the grid for your working area. You use this dialog box to set grid properties for both the schematic page grid and the part and symbol grid.

Use this control... To do this...

Visible

Specify whether the schematic page or part's grid is visible or hidden on the screen.

Grid Style

Specify whether the grid appears as grid dots or lines in the editor.

Grid spacing

Specify the grid spacing on the schematic page as a fraction of pin-to-pin spacing.

For example, a setting of 1/2 specifies that the grid spacing on the schematic page is set to exactly half the specified pin-to-pin spacing.

Pointer snap to grid

Specify whether the pointer snaps to the grid in the editor. This check box is selected by default.

Fine

(only for schematic page editor)

Specify whether connectivity (part, bus) and drawing objects, like Line, Polyline, Text, Rectangle, Ellipse, Arc, and Picture can be placed and moved on the fine grid. For description of various scenarios for this option, see Customizing placement and movement of objects on the schematic.

This setting is saved in the CAPTURE.INI file and it is used whenever you start the next Capture session.

Coarse

(only for schematic page editor)

Specify whether connectivity and drawing objects can be placed and moved on the coarse grid. For description of various scenarios for this option, see Customizing placement and movement of objects on the schematic.

This setting is saved in the CAPTURE.INI file and it is used whenever you start the next Capture session.

Master

(only for schematic page editor)

Specify whether connectivity and drawing objects can be placed and moved on the master grid, if Pointer snap to grid check box is selected. This setting is equivalent to the Snap To grid toolbar state .

Specify whether connectivity and drawing objects can be placed and moved on the fine grid, if Pointer snap to grid check box is not selected. This setting is equivalent to the Snap To grid toolbar state .

For description of various scenarios for this option, see Customizing placement and movement of objects on the schematic.

This setting is saved in the CAPTURE.INI file and it is used whenever you start the next Capture session.
Ensure that the Pointer snap to grid check box is selected and the Connectivity Elements is set to Coarse while placing connectivity objects. Otherwise, your part pins may be placed on the fine grid, making it difficult to connect them properly.
When you place a part on fine grid, it remains on fine grid through any cut-and-paste and drag-and-drop operations.

Miscellaneous tab

Use these options to specify miscellaneous options in Capture.

Use this control... To do this...

Fill Style

Specify a fill pattern for rectangles, ellipses, and polygons.

Line Style

Specify line style for lines, polylines, rectangles, ellipses, and arcs.

Line Width

Specify line width for lines, polylines, rectangles, ellipses, and arcs.

Color

Specify the color of lines, rectangles, and ellipses. Polylines and arcs use the default color of objects set in the Colors tab. This option only applies to lines, rectangles, and ellipses in the schematic page editor.

This color is not the default color, but can be set to use the default color. Objects placed while this option is not set to the default color, won't use the default color. Changing this option won't change the color of objects already placed in the schematic page editor.
You can change the fill style, line and width style, and color on individual objects using the Properties command on the Edit menu.

Junction Dot Size

Specify the dot size as Small, Medium, Large, and Very Large. This will increase or decrease the size of the dots created when a wire is connected to another wire.

Project Manager and Session Log

Specify the font for the session log. If you click on this box, a standard Windows Font dialog box for font selection appears. This option is neither a schematic page nor a part editor option.

Text Rendering

Render TrueType fonts with strokes

Specify that text appears as a series of lines, connected to resemble the outlines of the corresponding TrueType letters or numbers they represent.

Fill text

Specify that text outlines be filled in.

Auto Recovery

Enable Autorecover

Enable or disable auto recovery. If the option is checked, then auto recovery is enabled.

Update every N minutes

Specify the time interval in minutes (where N is the number of minutes) after which Capture performs an auto-save.

Auto recovery is not an automatic saving feature. If you intentionally exit Capture without first saving your changes, they will be lost. Autorecovered files are automatically deleted when you exit Capture normally.

Auto Reference

Automatically reference placed parts

(Default: ON)

Enable automatic part referencing. When a part is placed on the schematic page, the next available reference designator will automatically be assigned. Disabled, parts placed on the schematic will be assigned the reference designator found in the library. For example: U?A or JP?. This is the default selection.

You can choose to perform design level annotation by selecting the Design Level (Only PCB Designs) option. This option is not selected by default. This option should be used for PCB Designs only. For more information on Design Level Annotation, see Table 8-2: Design Level Annotation table.

The Auto Reference feature should be used to provide unique part references for simulation, and is not intended to replace the packaging process for a PCB design. For packaging you should Annotate your design.

Preserve reference on copy

Enable part references to be preserved while pasting a part to a schematic page. When you copy a part and paste it on a schematic page, the part will retain the same reference designator as that of the copied part. But, if you place a new part on a schematic page, Capture will assign the reference designator found in the library. For example: U?A or J?P.

This option is not supported for complex hierarchical designs.
You can select only one option at a time.

Depending on the check box selection state, the following scenarios are possible:

  • If both the check boxes are disabled:
    • the new part that you place on a schematic page will not be annotated.
    • the part references of the copied part will not be preserved while pasting that part on a schematic page.
  • If the Automatically reference placed parts check box is enabled:
    • the new parts that you place on a schematic page will be annotated.
    • the part references of the copied part will not be preserved while pasting that part on a schematic page, rather they will be incremented.
  • If the Preserve reference on copy check box is enabled:
    • the new part that you place on a schematic page will not be annotated.
    • the part references of the copied part will preserved while pasting that part on a schematic page.

Intertool Communication

Enable intertool communication

(Default: OFF)

Enable intertool communication with other OrCAD products such as Simulate or Layout. For more information about intertool communication, see Intertool communication. This option is not specific to either the schematic page editor or the part editor.

Wire Drag

Allow component move with connectivity changes

(Default: ON)

If this check box is selected or the toolbar button is in the Drag Connected Object state, then Capture allows you to drag and place the selected part or wire on the schematic, even if it results in connectivity changes. Also, Capture flags a warning with a changed cursor and will show the temporary markers.

If the check box is not selected or the toolbar button is in the Drag Connected Object state, then the selected part or wire attaches to the cursor and does not get placed on the schematic, if it results in connectivity changes. Also, Capture flags only a warning with a changed cursor and does not show the temporary markers.

Docking

Docking Place Part

(Default: ON)

If this option is checked, the dockable Place Part dialog is invoked when you select the Place Part command. Unchecking this option will ensure that the modal Place Part dialog displays.

You need to restart Capture to make changes to this option effective.

IREF Display Property

Global Visibility

(Default: ON)

Checking this option ensures that the intersheet references are visible. Unchecking this option will hide the intersheet references.

If you un-check this option (to hide the intersheet references in a design), and then run the Intersheet References command, the intersheet references will be displayed on the relevant pages of the design. If you then open the Miscellaneous tab, notice the Global Visibility option is checked.

Place Part

Refresh part on selection

(Default: OFF)

If this option is checked, then the library parts are updated in the Place Part dialog. Unchecking this option ensures that the library parts are not updated in the Place Part dialog.

Pan and Zoom tab

Use these options to specify panning and zooming factors. Set them separately for the schematic page editor, and the part and symbol editor.

Use this control... To do this...

Zoom Factor

Specifies the zoom factor for the editor.

The zoom factor can be any number between 1 and 10.

Auto Scroll Percent

Specifies how much of the schematic page or part scrolls across the screen when the pointer drags a selected object into the border area of the editor.

Select tab

Use these options to specify selection factors.

Use this control... To do this...

Area Select

Specify whether objects are selected when the selection area border intersects them, or only when they are completely enclosed in the selection area.

If the Fully Enclosed option is selected and you select an object on a schematic page, make sure that you select the object along with its name and number. Otherwise, the object does not get selected.

Maximum number of objects to display at high resolution while dragging

Specify the maximum number of objects that are visible at high resolution while performing a drag-and-drop operation. When you drag a number of objects greater than this value, a rectangular placeholder appears in lieu of the selected objects.

Show Palette

Specifies whether the tool palette is visible or hidden.

Text Editor tab

Use these options to specify the text settings like syntax highlight colors.

Use this control... To do this...

Syntax Highlighting

Displays the current colors for VHDL and Verilog keywords, comments, and quoted strings. Select one of the color buttons to display the standard Windows Color dialog box. In the Color dialog box, you can change the color of the selected language element.

Current Font Setting

Displays the current settings of the font item selected in the Set Font For option. The settings displayed are the font, font size, style, effects, and color.

Set

Display the standard Windows Font dialog box for setting font options. The settings apply to the selected font item only.
Be sure to use a monospaced font (for example, Courier) as the default font for the text editor or the source editor. If you use a true-type font, the editor may distort the appearance of the text, making it difficult to read.

Tab Setting

Specify the spacing between tabs in terms of character spaces for the text editor. The range is limited to 1-100.

This tab setting is stored in the CAPTURE.INI file. Capture will ignore existing CAPTURE.INI files that specify the tab setting in inches and will reset spacing to a default of four character spaces.

Highlight Keywords, Comments, and Quoted Strings

Specify that Capture highlight all VHDL or Verilog keywords, comments, and quoted strings in the active file.

Show line numbers

Specify that the text editor display line numbers in text files

Save text files on deactivate

Specify that any open text files are saved in their current state whenever the text editor window loses focus

Auto reload text files

Specify that the text editor reload text files automatically when there is a more recent version of the file as a result of a Capture operation (such as netlist generation).

Save text files before running tools

Specify that the text editor save any open text files before running any Capture tools (such as design rules check or netlist generation).

Reset

Reset all the tab options to Capture's default values.

Board Simulation tab

Use these options to specify the hardware development language used for board simulation.

Use this control... To do this...

VHDL

Specify that Capture use VHDL for the board simulation netlist and testbench.

Verilog

Specify that Capture use Verilog for the board simulation netlist and testbench.

Print dialog box

To open this dialog

Choose Print (see Print command) from the File menu.

Click the Setup button to go to the Print Setup dialog box and check settings before you print. All settings you choose (except the number of copies) are saved to CAPTURE.INI and will become the default when you restart Capture.
Use this control... To do this...

Printer

Displays the active printer and printer connection.

Scale

Specify the scaling factor to print by, or let Capture automatically scale to the specification.

  • Scaling to paper size - Forces Capture to scale the printing job to the page size specified in the Page Size tab in the Schematic Page Properties dialog box. Use the Page Size tab in the Design Template dialog box on the Options menu to reset the Custom page size.
  • Scale to page size - Forces Capture to scale the printing job to the page size specified by the Page size option in the Print dialog box.
  • Scale - Specifies the scaling factor to print by, or lets Capture automatically scale to the specified scale.

Page size

If Scale to page size is selected, select the page size to which the image will be scaled. Choose one of the standard page sizes, or Custom. These sizes are defined in the Schematic Page Properties dialog box, in the Page Size tab.

Print offsets

Specifies horizontal and vertical printing offsets in inches or millimeters (mm) depending on the setting you’ve chose in the Design Template dialog box. Capture centers the page horizontally and vertically when both check boxes are selected.

Your entire schematic page will be output to the printing or plotting device, regardless of the use of offsets. The following rules define the number of output pages that will be printed or plotted:

  • The device and its driver determine the dimensions of the printed page area.
  • The number of pages is calculated from the physical dimensions of the schematic page and the driver-provided area dimensions.
  • A positive offset shifts the entire schematic page to the right in the X direction, and down in the Y direction. Additional pages are output as necessary so the entire schematic is printed. There is no truncation.
  • A negative offset shifts the schematic page left, and up. The effect of a negative offset is to start the drawing on a “previous” page. Previous pages are “prepended” so drawing can start at the starting portion of the schematic. There is no truncation.
  • Only the number of pages required to print or plot the schematic page will be printed. Extra, blank pages are omitted.

Print option

Specify whether you want to print instances or occurrences of a page.

  • Inst. Mode (Instance mode) - Enables you to print only the instances of a page in a schematic. This option is selected by default.
  • Occ. Mode (Occurrence mode) - Enables you to print multiple occurrences of a page in a schematic.

Print quality

Specify the resolution of the print. Choose a setting from the drop-down list.

Copies

Specify the number of copies to print.

Print to file

Print the object to a file. If you select this option, the Print to File dialog box appears after you click OK.

Print all colors in black

Causes difficult-to-read colors to print in black.

Collate copies

Print copies organized in order of page numbers

Print area

When a specific print area is set for the schematic page and this option is selected, the print output is the print area of the schematic page. Clear this check box to print the entire schematic page.

When Print area is selected, all print options except Print quality, Copies, Print to file, and Print all colors in black are unavailable. Output of selected print area is zoomed in and centered.

Include pages outside hierarchy

Specifies to also print pages in the design that are not included in the root hierarchy. If you do not select this option, only those files included in the root hierarchy will print.

Include referenced pages in other libraries or designs

Specifies to also print pages outside of the design that the root hierarchy references. If you do not select this option, only the files in the design’s root hierarchy will print.

Print statistics
  • Printed pages per document page - Specifies the number of horizontal and vertical pages needed to print a document. If a schematic page (document page) takes more than one page to print out, Capture reports the total number of pages under the Total column heading. Horizontal and Vertical refers to the pages that will make up the printed schematic page. For example, a schematic page may take four pages to print, so the Total is 4. Depending on physical shape of the design, the Horizontal may be 2 and the Vertical may be 2 (2 x 2), or the Horizontal may be 4 and the Vertical may be 1 (4 x 1).
  • Maximum page size for selected printer - These dimensions identify the printable page area of the printer and are dependent on the printer and paper size.
  • Size from schematic page properties - Specifies the dimensions of the page size selected on the Page Size tab of the Schematic Page Properties dialog box.
  • Size of actual printout - Specifies the scaled document size as it changes with different settings in the Scale options or when you change the page orientation in the Print Setup dialog box. The Maximum size for the page layout, Size from schematic page properties, and Size of actual printout dimensions are shown in inches or millimeters, depending on the setting you’ve chose in the Design Template dialog box.

Setup

Display a standard Windows dialog box to set printer or plotter configuration.

The Print statistics section of the Print and Print Preview dialog boxes reports the number of horizontal and vertical pages it takes to print out the selected document. If the schematic page you want to print takes a two-page layout as shown here:

You would see this in the Printed pages per document page statistics:

When printing a multi-page schematic, make sure that the pages do not have multiple Title Blocks with different page numbers. Otherwise, the pages will not be printed in the correct order. If you change the page numbers in the Title Blocks manually, then make sure that the Do not change the page number check box is checked in the Annotate dialog box.

Print Preview and Print Setup dialog boxes

To open this dialog

Choose Print Preview (see Print Preview command) from the File menu.

Click the Setup button to go to the Print Setup dialog box before you print. All settings you choose (except the number of copies) are saved to CAPTURE.INI and will become the default when you restart Capture.
Use this control... To do this...

Printer

Displays the active printer and printer connection.

Scale

Specify the scaling factor to print by, or let Capture automatically scale to the specification.

  • Scaling to paper size - Forces Capture to scale the printing job to the page size specified in the Page Size tab in the Schematic Page Properties dialog box. Use the Page Size tab in the Design Template dialog box on the Options menu to reset the Custom page size.
  • Scale to page size - Forces Capture to scale the printing job to the page size specified by the Page size option in the Print dialog box.
  • Scale - Specifies the scaling factor to print by, or lets Capture automatically scale to the specified scale.

Page size

If Scale to page size is selected, select the page size to which the image will be scaled. Choose one of the standard page sizes, or Custom. These sizes are defined in the Schematic Page Properties dialog box, in the Page Size tab.

Print offsets

Specifies horizontal and vertical printing offsets in inches or millimeters (mm) depending on the setting you choose in the Design Template dialog box. Capture centers the page horizontally and vertically when both check boxes are selected.

Your entire schematic page will be output to the printing or plotting device, regardless of the use of offsets. The following rules define the number of output pages that will be printed or plotted:

  • The device and its driver determine the dimensions of the printed page area.
  • The number of pages is calculated from the physical dimensions of the schematic page and the driver-provided area dimensions.

  • A positive offset shifts the entire schematic page to the right in the X direction, and down in the Y direction. Additional pages are output as necessary so the entire schematic is printed. There is no truncation.
  • A negative offset shifts the schematic page left, and up. The effect of a negative offset is to start the drawing on a “previous” page. Previous pages are “prepended” so drawing can start at the starting portion of the schematic. There is no truncation.
  • Only the number of pages required to print or plot the schematic page will be printed. Extra, blank pages are omitted.

Print option

Specify whether you want to print instances or occurrences of a page.

  • Inst. Mode (Instance mode) - Enables you to print only the instances of a page in a schematic. This is the default option.
  • Occ. Mode (Occurrence mode) - Enables you to print multiple occurrences of a page in a schematic.

Print quality

Specify the resolution of the print. Choose a setting from the drop-down list.

Copies

Specify the number of copies to print.

Print to file

This option is not available in Print Preview. If you want to print to file, use the Print dialog box.

Print all colors in black

Causes difficult-to-read colors to print in black.

Collate copies

Print copies organized in order of page numbers

Print area

When a specific print area is set for the schematic page and this option is selected, the print output is the print area of the schematic page. Clear this check box to print the entire schematic page.

When Print area is selected, all print options except Print quality, Copies, Print to file, and Print all colors in black are unavailable. Output o selected print area is zoomed in and centered.

Include pages outside hierarchy

Specifies to also print pages in the design that are not included in the root hierarchy. If you do not select this option, only those files included in the root hierarchy will print.

Include referenced pages in other libraries or designs

Specifies to also print pages outside of the design that the root hierarchy references. If you do not select this option, only the files in the design’s root hierarchy will print.

Print statistics
  • Printed pages per document page - Specifies the number of horizontal and vertical pages needed to print a document. If a schematic page (document page) takes more than one page to print out, Capture reports the total number of pages under the Total column heading. Horizontal and Vertical refers to the pages that will make up the printed schematic page. For example, a schematic page may take four pages to print, so the Total is 4. Depending on physical shape of the design, the Horizontal may be 2 and the Vertical may be 2 (2 x 2), or the Horizontal may be 4 and the Vertical may be 1 (4 x 1).
  • Maximum page size for selected printer - These dimensions identify the printable page area of the printer and are dependent on the printer and paper size.
  • Size from schematic page properties - Specifies the dimensions of the page size selected on the Page Size tab of the Schematic Page Properties dialog box.
  • Size of actual printout - Specifies the scaled document size as it changes with different settings in the Scale options or when you change the page orientation in the Print Setup dialog box. The Maximum size for the page layout, Size from schematic page properties, and Size of actual printout dimensions are shown in inches or millimeters, depending on the setting you’ve chose in the Design Template dialog box.

Setup

Display a standard Windows dialog box to set printer or plotter configuration.

Print Setup dialog box

To open this dialog

choose the Print Setup (see Print Setup command) from the File menu.

OR

Click the Setup button on the Print dialog box or Print Preview and Print Setup dialog boxes.

The Print Setup dialog box is a standard windows dialog box for configuring your printer or plotter. Use it to choose a printer, paper source, and orientation before printing. For more information on setting up printers and plotters, refer to the documentation for your configured printer driver.

Many times, the options for your printer are not available in the standard setup dialog box. If you do not find the options you need, try the printer setup in the Windows Control Panel.

Print to File dialog box

To open this dialog

In the Print dialog box, select the Print to File option and then click OK.

Use this control... To do this...

Output file name

Specify the name of the output file.

Programmable Logic Project Wizard dialog box

Programmable logic project for designs may include Verilog or VHDL models as part of the structure. Projects of this nature will often use simulation and synthesis tools as part of the design flow. When you create a programmable logic project, certain folders are added to the project. These are discussed in Working with the project manager.

To create a programmable logic project:

  1. Select the logic vendor and target family for the project (for example, Actel, Altera, and Xilinx family).
  2. Click the Finish button.

Propagation Delay dialog box

Use this dialog box to specify a pin-pair and select valid minimum and maximum value for the PROPAGATION_DELAY property.

The PROPAGATION_DELAY property has the following syntax:

<Pin_pair>:<min_value>:<max_value>

To open this dialog

While editing the PROPAGATION_DELAY property in the Property Editor, choose Invoke UI from the Edit menu press CTRL+U.

OR

Right-click the grid corresponding to the PROPAGATION_DELAY property and select Invoke UI from the popup menu.

Use this control... To do this...

Pin Pair

Applies Min and/or Max delay constraint to various pin-pairs. This value may be set to one of the following:

  • Longest/Shortest pin-pair—Minimum delay is applied to the shortest pin-pair and maximum delay is applied to the longest pin-pair.
  • Longest/Shortest Driver/Receiver—Minimum is applied to the shortest Driver/Receiver pin-pair and maximum is applied to the longest Driver/Receiver pin-pair.
  • All Drivers/All Receivers—Min/Max constraints apply to all Driver/Receiver pin-pairs.

Min

Specifies the minimum allowable propagation delay/length for the pin-pairs.

Min Rule

Specifies whether the minimum allowable propagation delay is measured as DELAY in ns, %MANHATAN, or LENGTH in mills (mils), micron (um), millimeter (mm), centimeter (cm), and inches (in).

Max

Specifies the maximum allowable propagation delay/length for the pin-pairs.

Max Rule

Specifies whether the maximum allowable propagation delay is measured as DELAY in ns, %MANHATAN, or LENGTH in mills (mils), micron (um), millimeter (mm), centimeter (cm), and inches (in).

Add Pin Pair

Displays the Create Pin Pairs dialog box. Use this dialog box to define a pin-pair.

Keyboard shortcut: ALT, A

Delete Pin Pair

Deletes the pin-pair corresponding to the selected row.

Keyboard shortcut: ALT, D

OK

Performs syntax checking and if the syntax is correct assigns the PROPAGATION_DELAY property on the selected net.
You can use the User Properties dialog box to assign the PROPAGATION_DELAY property to all the bits of a bus at the same time. Make sure that you use the correct syntax for specifying a value for the PROPAGATION_DELAY property. The syntax is:
<Pin_pair>:<min_value>:<max_value>

The pin-pairs can only be:

Properties dialog box

Use the dialog box to access information about the current project, or the file currently selected in the project manager window. You can also change the description of a file.

To open this dialog

Choose Properties (see Properties command) from the Edit menu or from the pop-up menu.

Use this tab... To do this...

General tab

Provide information about the file name, size, and the date it was last modified. For more information, see General tab

Type tab

Specify the type of the file, such as schematic or simulation model. For more information, see Type tab.

Project tab

Specify project options. These options include project type, vendor, and family. For more information, see Type tab.

General tab

Use this control... To do this...

File name

Displays the name of the file currently selected in the project manager window.

Last modified date

Displays the date that the file was last modified.

Size

Displays the size (in bytes) of the file currently selected in the project manager window.

Type tab

Use this control... To do this...

File type drop-down list

The drop-down list provides a list of file descriptions. The file description of the file that is currently selected in the project manager window appears in the window. Select another file description from the drop list to change the file type of the file currently selected in the project manager window.

PSpice Part Search dialog box

Use this dialog box to place PSpice Parts on the schematic page by searching them in the libraries using PSpice Part Search.

To open this dialog

Select Place – PSpice Component – Search.

Use this control... To do this...

Category View

Hide Categories View/Show Categories View

Toggle Hide Categories View or Show Categories View to hide or unhide the Category View.

Search Online

Opens new window in Capture for searching PSpice models in OrCAD Capture Marketplace

Categories tab

Displays PSpice parts in categories defined by PSpice parts function

Library tab

Displays PSpice parts in the libraries they are associated to

Search Window View

Search text box

Enter the search text to search for PSpice parts in the PSpice Part Search database

Search drop-down list

Provides option to search in selected category or all categories

Symbol Viewer

Displays symbol of the selected part

Part Table View

Part Name

Displays part name of the PSpice part

Description

Displays brief description of the PSpice part

Symbol Library

Displays library path of the selected PSpice part


Return to top