05 - Working with Database Parts

Prerequisites to Database Part Placement

Before you place a database part, you need to do the following tasks:

• Locate a part in your parts database.
  • Using Explorer
  • Using Query Feature

When you place a database part, CIS includes all database part properties to be transferred.

Using Explorer to Locate a Database Part

You can use Explorer to locate a particular part in your database.

To locate a database part with the explorer, do the following:

1. From the schematic page editor’s Place menu, choose Database Part. CIS displays the explorer window.
2. In the Explorer window, choose the Explore tab. The drum icon (labeled Benchacc in this example) represents the part database.

3. Choose  or double-click the drum icon, to expand the database into the configured part tables. Similarly, choose  on the table to expand the tree to display the first-level part type folders.

   If you want to display the whole part tree structure, from the View menu, choose Expand Part Tree.

4. Locate the part you want to place. When you open a part type folder at any given level, the database parts at that level are displayed in the database parts window.
   

Using the Query Feature to Locate Database Parts

You can also use the query feature in the CIS explorer window to locate all parts in the database that fit a set of criteria. This is useful when you want to view all the available parts that match a set of attributes. To use the query feature, you must first create the query criteria, then execute the database search. Additionally, you can:

• Save and retrieve queries.
• Modify saved queries.
• Delete saved queries.

Creating and Executing a Non-relational Query

Capture CIS allows you to create non-relational queries on a flat structure database. To do so, follow the steps:

1. From the schematic page editor’s Place menu, choose Database Part. CIS displays the CIS explorer window.
2. In the Explorer window, choose the Query tab.
3. In the first cell in the Property column, type in the name of a property or choose one from the cell’s drop-down list.
   
4. In the first cell in the Compare column, type in a logical operator or choose one from the cell’s drop-down list.
5. In the first cell in the Value column, enter a value. If you’re using the equal to (=) logical operator, you can use wildcard characters for the value: an asterisk (*) matches a group of characters, and a question mark (?) matches any single character.
   Repeat steps step 3 through step 5 as necessary to construct subsequent rows of search criteria. You can delete a query row by selecting the row and then pressing Delete. Since a database search identifies only those parts that meet all the search criteria, you can use additional rows of criteria to pinpoint specific parts.
6. To perform the query, press Enter or choose Re-search Database from the Update menu. CIS displays the results in the database parts window.

Saving and Retrieving a Non-relational Query

OrCAD X Capture CIS enables you to save your queries and retrieve them in subsequent Capture CIS sessions.

To save a query, do the following:

1. Create a query.
   
2. Specify a name for the query in the Select a Query combo box.
3. Click Save Query. The query is saved and the query name appears in the Select a Query combo box.

To retrieve a saved query, in the Query tab of the Explorer window, select the query you want to retrieve from the Select a Query combo box. The query definitions for the selected query appear under the respective column headers in the Explorer window.

Modifying a Saved Query

You can change the existing query definitions in a saved query and use it later.

To modify an existing saved query, do the following:

In the Query tab of the Explorer window, select the query you want to modify from the Select a Query combo box. The query definitions appear under the respective column headers in the Explorer window.

1. Change the query definitions as desired.
2. Click Save Query. The query is updated.

Deleting a Saved Query

You can delete an existing saved query.

To delete an existing saved query, do the following:

1. In the Query tab of the Explorer window, select the query you want to delete from the Select a Query combo box. The query definitions appear under the respective column headers in the Explorer window.
2. Click Delete Query. The query along with the query definitions are deleted from the CISQuery.txt file and the query name does not appear in the Select a Query combo box.

Creating and Executing a Relational Query

Capture CIS also allows you to create non-relational queries on a flat structure database. However, the relational view will be enabled in CIS explorer only if at least one relation is defined in CIS configuration.

1. From the schematic page editor’s Place menu, choose Database Part. CIS displays the CIS explorer window.
2. In the Explorer window, choose the Query tab.
3. Select the Relational Query checkbox.

4. In the Select a Table drop-down list, choose a primary table to query.

   The drop-down list will show only the tables for which relational query has been defined.

   When you select particular table for running a query, all the properties of that table are available in the property tab to formulate a query. If you select "All Tables" the union of the properties of all the relational tables is available for forming the query.

5. In the Property column, type in the name of a property or choose one from the cell’s drop-down list.
6. In the Compare column, type in a logical operator or choose one from the cell’s drop-down list.
7. In the Value column, enter a value. If you’re using the equal to (=) logical operator, you can use wildcard characters for the value: an asterisk (*) matches a group of characters, and a question mark (?) matches any single character.
   Repeat steps step 3 through step 5 as necessary to construct subsequent rows of search criteria. You can delete a query row by selecting the row and then pressing Delete. Since a database search identifies only those parts that meet all the search criteria, you can use additional rows of criteria to pinpoint specific parts.
8. To execute the query, press Enter or choose Re-search Database from the Update menu. CIS displays the results in the database parts window.

Placing a Database Part

After locating the database part from the local part database, you can place it on your schematic page.

Any properties specified during configuration as transferable are copied to the placed part and are present in the placed part properties.

CIS sets the appropriate property visibility. If the property is set to Visible and exists in the library, CIS uses the property position defined in the library; otherwise, CIS displays the property in a default position. If you change the position of a property in the part editor, any subsequent updates to the part (using the Link Database Part command) retain the new position.

You can also use the library convert feature to hold two different orientations of the part, one for the normal orientation and one for the 90-degree rotation.

Setting Path for Custom Libraries

Before placing database components, you should make sure that path for all the libraries including custom libraries, is initialized. There are three ways to initialize a library path:

• Add a library from the custom library path in the Place Part dialog box and restart Capture. When you restart Capture, the newly modified Capture.ini file will be read.
• Manually add path of the custom libraries to the Capture.ini file before opening Capture.
• Use the OrCAD X INI File Administrator utility to define the paths for custom libraries.

To place a database part on your schematic, do the following:

1. In the database parts window, select the part you want to place.
2. If the database part has multiple schematic parts associated with it and you want to select a different schematic part name, select one from the drop-down list for the Schematic Part property name.
   
3. If the database part has multiple PCB footprints associated with it and you want to select a different PCB footprint name, select one from the drop-down list for the PCB Footprint property name.
4. If you want to override the default visibility settings of one or more transferable part properties, change the settings in the visibility window. There are four possible visibility settings:
   • CIS displays the property with the part on the schematic page
   • CIS does not display the property with the part on the schematic page.
   • CIS does not modify the property visibility. If the property does not exist, it is set to invisible.
   • CIS does not allow this property to be set as visible on schematic pages.
5. Start placing the part by doing one of the following:
   • In the database parts window, double-click your selected part.
   • From the Right-Click Pop-Up menu, choose Place Database Part.
6. Click to place the part. Press Esc when you’re finished placing instances of this part.

Browsing Part Properties

Database parts may include browsable properties. These properties actually specify links to documents or websites. CIS allows you to browse properties for which the Browsable option was set during configuration.

→ To browse a database part property, click the database part property you want to browse in the database parts window. The cursor turns into a hand when you point at a browsable property.

Since the browsing feature is generic, you can view virtually any kind of data. You can include references to your component datasheets on your company’s intranet, as Word files, Acrobat files, or any other format. For example, you may want to view package drawings, mechanical models, simulation models, and so on.

CIS launches the appropriate browser based on the value of the part property.

CIS starts your default web browser and displays the web page for that URL.

Creating a New Database Part

Almost every design will use some new parts that aren’t in your part database and do not have a company part number. CIS lets you create a new part while you’re working and save it to the database. This allows you to continue working without having to stop for the part approval process. When you save a temporary part to your database, CIS can automatically assign a temporary part number and track the part for you in the part manager. Later, if the part is approved and assigned a company part number, CIS can automatically update your design with the new part information. 

You can create new database parts using one of the following methods:

• Using Local Part Database
• Using a Part Placed on a Schematic Page

Using the Local Part Database

You can create new database parts using parts that are already stored in your database. Once you have selected and altered an existing database part, you can store it as a temporary part in your database and place instances of the new part on schematic pages.

To derive a new part for the part database, do the following:

1. If a schematic page is not already open and active, open a schematic page.
2. From the Place menu, choose Database Part. CIS displays the CIS explorer.
   
   
3. Use the explore and query features to locate the part you want to use as the basis for creating your new database part. 
4. Select the desired part in the database parts window.
5. From the Edit menu, choose Derive New Database Part. CIS displays the New Database Part dialog box.
   
   

6. Enter the appropriate values for the new part’s database properties in the Contents column. You cannot change the selected table in the Save Part To area. This is because you are deriving the new part from a placed part that is already in your part database, so the new part is automatically placed in the same table as the existing database part.

   If you have selected Assign Temporary Part Numbers Automatically in the configuration, a temporary part number is already assigned which you cannot modify.

7. Modify the visibility settings for each property as desired.
8. If you want to choose alternate schematic parts or footprints for the new database part, do the following:
   1. Click the Browse button in the Schematic Part area to choose alternate schematic parts or in the Footprint area to choose alternate footprints. CIS displays the Select Schematic Part or Select Footprint dialog box.
      
      
   2. If you want to include the library name with the selected schematic parts or footprints, select the Attach the Library Name option. You can include the library name to avoid confusing the schematic part or footprint name with an identically named one in a different library.

   3. In the Schematic Part or the Footprint list, select a part or a footprint. The part or footprint displays in the preview window.

      If you know what library your footprints or schematic parts are stored in, highlight only that library in the Configured Libraries list. This will greatly reduce the number of schematic parts you have to scroll through to find part or footprint names.

      Only select a schematic part from your own custom libraries; do not select a part from the libraries that are supplied with Capture (resource libraries). Resource libraries are often changed by upgrades to new versions of Capture. If the name or path of the schematic part you select is changed during an upgrade, it will become invalid for all your database parts.

      If you are deriving a new mechanical (non-electrical) part and choosing an alternate schematic part, you must choose a schematic part with no pins. If mechanical parts with pins are placed in a design, they will invalidate netlists generated from that design.

   4. Click the Add button to move the schematic part or footprint to the Selected Schematic Parts or Selected Footprints list. You can remove it from the list by selecting it and clicking the Remove button.
   5. Repeat steps step c and step d until you have selected all the schematic parts or footprints that you want to be available for use with the database part.
   6. If you selected more than one schematic part or footprint, use the up and down arrows to arrange the order of the parts or footprints. The top one will be the default value for the database part. The order of the whole set determines the order in which they will display in the scroll-down list of the Schematic Part or PCB Footprint property value cells of the CIS explorer’s database parts window.
      
      
      
   7. Click OK. CIS returns you to the New Database Part dialog box.

9. Click the Place Part button. The dialog box closes, the new part is added to the part database, and you are returned to the schematic page with the pointer in place part mode.

   After the new part is added to the database, you must have administrative privileges for the database to modify the properties that you set above.

10. Click to place the part. Press Esc when you are finished placing instances of the part.

Using a Part Placed on a Schematic Page

You can create new database parts using parts that you have already placed on schematic pages. While you are deriving a new database part, you can change the values and visibility settings of the database part properties.

By default, CIS does not automatically copy all placed part properties to the part database. The properties that are automatically transferred have all three of the following characteristics:

• They are mapped to database part properties in the database configuration.
• They have been set to transfer to designs in the database configuration.
• They have a value for the placed part.

If you want other property values to be added to the database, you can manually add them during this procedure, but only if the property is mapped in the database configuration.

As soon as the new part is stored in the database, you can place instances of the part on schematic pages. The part will remain a temporary part, however, until your database administrator assigns a permanent part number.

To derive a new part from a database part, do the following:

1. Open the schematic page that contains the placed part you want to use to derive a new database part.
2. Select the placed part.
3. From the Edit menu, choose Derive Database Part. CIS displays the New Database Part dialog box.
   
   

4. In the Save Part To area, choose the database table in which you want to save the new database part.

   If you are deriving the new part from a placed part that is already in your part database, the new part is automatically placed in the same table as the existing database part. CIS will not allow you to select a different table.

5. If you want to change the value of a database property, enter the new value in the Contents column.

   If you have selected the Assign Temporary Part Numbers Automatically option in the configuration, a temporary part number is already assigned which you cannot modify.

6. Modify the visibility settings for each property as desired.
7. If you want to choose alternate schematic parts or footprints for the new database part, do the following:
   1. Click the Browse button in the Schematic Part area to choose alternate schematic parts or in the Footprint area to choose alternate footprints. CIS displays the Select Schematic Part or Select Footprint dialog box.
      
   2. If you want to include the library name with the selected schematic parts or footprints, select the Attach the Library Name option. You can include the library name to avoid confusing the schematic part or footprint name with an identically named one in a different library.

   3. In the Schematic Part or the Footprint list, select a part or a footprint. The part or footprint displays in the preview window.

      If you know what library your footprints or schematic parts are stored in, highlight only that library in the Schematic Part Libraries or Configured Libraries list. This will greatly reduce the number of schematic parts you have to scroll through to find part or footprint names.

      Only select a schematic part from your own custom libraries; do not select a part from the libraries that are supplied with Capture (resource libraries). Resource libraries are often changed by upgrades to new versions of Capture. If the name or path of the schematic part you select is changed during an upgrade, it will become invalid for all your database parts.

      If you are deriving a new mechanical (non-electrical) part and choosing an alternate schematic part, you must choose a schematic part with no pins. If mechanical parts with pins are placed in a design, they will invalidate netlists generated from that design.

   4. Click the Add button to move the schematic part or footprint to the Selected Schematic Parts or Selected Footprints list. You can remove it from the list by selecting it and clicking the Remove button.
   5. Repeat steps step c and step d until you have selected all the schematic parts or footprints that you want to be available for use with the database part.
   6. If you selected more than one schematic part or footprint, use the up and down arrows to arrange the order of the parts or footprints. The top one will be the default value for the database part. The order of the whole set determines the order in which they will display in the scroll-down list of the Schematic Part or PCB Footprint property value cells of the CIS explorer’s database parts window.
      
   7. Click OK. CIS returns you to the New Database Part dialog box.
8. Click the Derive Part button. The part is added to the part database with the automatically assigned part number.

Linking a Placed Part to a Database Part

You can use the Link Database Part command from the part manager or the schematic page editor to assign a database part (and the associated transferable properties) to one or more placed parts. You can also specify whether you want to:

• replace the symbol, reference designator, and all the properties of the placed part with that of the database part.
• replace the symbol and all the other properties of the placed part with that of the database part, but retain the placed part reference designator.
• replace all the properties of the placed part with that of the database part, but retain the placed part symbol and the reference designator. 

OrCAD X Capture CIS allows you to link selected part occurrence(s) or a part with multiple occurrences to a database part.  It includes the following tasks:

• Setting Linking Preferences
• Linking Parts using Part Manager
• Linking Parts using Schematic Page Editor
  
  

Setting Linking Preferences

You can set preferences for linking a placed part to a database part by using the Extended CIS Linking command.

To set link preferences, do the following:

1. From the Capture CIS window, select the Options menu, point to CIS Preferences, and choose the Extended CIS Linking command or press SHIFT+E shortcut keys. The Extended CIS Linking dialog box appears.
   

   The Extended CIS Linking command is also accessible from the project manager and the schematic page editor.

2. Use the Extended CIS Linking dialog box to specify the following options:

   To...	Select...
   Retain the symbol and reference designator of the placed part and replace all the properties of the placed part with that of the database part	Preserve Reference Designator and Preserve Symbol check boxes.
   Retain the placed part symbol, but replace all the other properties of the placed part with that of the database part.	Preserve Symbol check box only.
   When you select the Preserve Symbol check box, the Preserve Reference Designator check box is selected automatically.
   Replace the symbol and all the other properties of the placed part with that of the database part, but retain the placed part reference designator.	Preserve Reference Designator check box only.

   The default behavior of OrCAD X Capture CIS is to replace the symbol, reference designator, and all the properties of the selected placed part with that of the database part.

3. Click OK to save the settings. The settings are saved in the CAPTURE.INI file. The next time you link a placed part to a database part these settings will be used.

   The link preferences can be changed any number of times during a Capture CIS session using the Extended CIS Linking command.

   Do not select the Preserve Reference Designator check box, if you are linking a placed part to a database part that differ in the number of components. Otherwise, the reference designators for the placed part will not be preserved after the linking is done.

   It is recommended that you set the linking preferences before you use the Link Database Part command to link a placed part to a database part.

Linking Parts using Part Manager

To link a placed part to a database part using the part manager, do the following:

1. Choose Tools - Part Manager - Open.  CIS displays the part manager window.
2. In the part manager, select a placed part or a group of placed parts. To select a group of parts, do one of the following
   • For a group of nonadjacent parts, hold down Control and click the parts.

   • For a group of adjacent parts, hold down Shift and click the first then the last part in the range.

     You can group similar parts in the part manager by sorting on one of the columns (for example, the Value column). Choose a column heading to sort the list by the information in that column; choose the same heading again to reverse the sort order.

3. From the Tools menu, choose Link Database Part.
   or
   Click the Link Database Part  toolbar button.

4. In the part database explorer:
   Double-click the database part you want.
   or
   Select the database part you want and, from the Update menu, choose Link Database Part.
   If the schematic part property for the placed part is different from that of the selected database part, CIS will highlight the database part’s row yellow when you select it in the database parts window.

   In the visibility window, CIS displays the values of the selected database part’s properties in the Database Contents column and the values of the placed part’s properties in the Schematic Contents column. If the value of placed part’s property is green, then it matches the value of the property for the database part. If the value of placed part’s property is red, then the value does not match that of the database part.

   CIS displays a warning message, if you select a database part to link to a group of placed parts whose part reference prefixes or values differ. CIS will, however, allow you to link a placed part to a database part with a different schematic part name.

   CIS links the database part to the placed part, and the appropriate properties are transferred.

   Because the schematic part used for the placed part will change, you must check the schematic page to make sure that you have correct connectivity when you are finished linking.

[Symbol Libraries]

Strict Cache Check=1

Linking Parts using Schematic Page Editor

To link a placed part to a database part using the schematic page editor, do the following:

1. Select one or more parts on a schematic page.
2. From the Edit menu, choose Link Database Part. CIS performs a database query, using the keyed properties for the database, then displays the results of the query in the database parts window.
   
   Keyed properties are defined in the database configuration. Generally, though, the Value property is the primary keyed property. The initial query searches for parts with a value matching that of the placed part. If you select several parts, CIS uses the keyed properties and part reference prefix of the first part in the group (from top left to bottom right) for the initial query.
   CIS also uses the configuration settings for Allowed Part Reference Prefixes and Part Reference Associations to filter the database for only those parts that apply to the reference prefix of the selected parts.
3. Select the database part you want to apply to the selected placed parts. You can also create a new query if the initial query did not locate the part of interest.

4. In the part database explorer, do one of the following:
   Double-click the database part you want.
   or
   Select the database part you want and, from the Update menu, choose Link Database Part.
   If the schematic part property for the placed part is different from that of the selected database part, CIS will highlight the database part’s row yellow when you select it in the database parts window.

   In the visibility window, CIS displays the values of the selected database part’s properties in the Database Contents column and the values of the placed part’s properties in the Schematic Contents column. If the value of placed part’s property is green, then it matches the value of the property for the database part. If the value of placed part’s property is red, then the value does not match that of the database part.

   The database part is linked to the placed parts, which also receive the transferable properties, including the part value. If any of the selected placed parts are multiple-part packages and have defined part references, CIS updates all other parts in the package at the same time. For example, if the selected placed part is U33B, CIS will update U33A, U33C, and any other parts in the package as well. If the selected placed part reference is undefined, only the selected part is updated.

   Because the schematic part used for the placed part will change, you must check the schematic page to make sure that you have correct connectivity when you are finished linking.

[Symbol Libraries]

Strict Cache Check=1

Linking Part Occurrence(s) to a Database Part

You can select whether you want to link all the occurrences of a selected part (s) or only the selected occurrence (s) of a part to a database part.

To link part occurrence(s) to a database part, do the following:

1. Select one or more parts on a schematic page or the part manager.
2. Right-click on the selection and choose Link Database Part from the pop-up menu.
3. If the selected part (s) has:
   • only a single occurrence in the design, then the part database explorer appears where you can select the database part to be linked to the selected part (s).
   • more than one occurrence in the design, then the Occurrence Level Settings dialog box appears.
     

1. Select Link to Selected Occurrences Only check box to link the database part to the part (s) you have selected on the schematic page or the part manager.
   or
   Select Link all Occurrences check box to link the database part to all the occurrences of the selected part (s) on a schematic page.

   CIS does not allow you to link a database part to part(s) in a group, which have multiple occurrences.

   
2. Click OK. The part database explorer appears where you can select the database part to be linked to the selected part (s). The settings are saved in the CAPTURE.INI file.

If you select the Do not show this dialog again check box, the Occurrence Level Settings dialog box will not be displayed the next time you link a part (s), which has multiple occurrences in a design. To display this dialog box again, you must change the following entry under the [Link Settings] section in the CAPTURE.INI file:

[Link Settings]

Show Occurrence Link Dialog=FALSE

to

[Symbol Libraries]

Strict Cache Check=1

Viewing Database Properties of a Placed Part

You can view a placed part’s local and Internet database properties right from the schematic page or the part manager, if the part has been added to the local part database. When you choose to view the part properties, CIS displays a read-only version of the CIS explorer with a comparison of the placed part’s properties to those of its linked database part. You can also use this part viewing capability to check the latest datasheet, stocking, and pricing information from the Internet.

To view a placed part’s database properties, do the following:

1. From the schematic page or the part manager, select the part for which you want to view database properties.

   On the schematic page, the selected part must be in your local part database for CIS to display part properties. If you attempt to view the database properties of a part not stored in your local part database, CIS will display the Local Part Database tab of the CIS Explorer window with no part information.

2. Select View - Database Part. CIS displays the CIS explorer window in View Database Part mode.

   The View Database Part mode is a read-only mode. For this reason, you cannot use the search or query functions of the explorer window to search for, place, or link a database part.

   CIS displays the database part property contents in the database parts window. In the visibility window, CIS displays both the contents of the database parts properties and the properties that have been transferred to the schematic. If the content of a schematic property is green, then it matches the content of the part database. If the content of a schematic property is red, then the contents do not match the part database.

Copying Part Properties Using Part Manager

You can also use the part manager to copy properties from one part to another (or to several others) in the design. CIS copies only those properties defined in the database configuration file as transferable.

To copy properties from one part to another, do the following:

1. Open the schematic design that contains the part properties you want to copy.
2. From the Tools menu, point to Part Manager, and choose Open. CIS displays the part manager, showing all parts in the design, sorted by part reference.
   
3. Select the part with the properties to be copied. You can use the Split command (from the part manager’s Window menu) to display two areas of the part manager. This can make copying properties from one part to another much easier (by dragging the part across split panes) if the two parts are widely separated in the part manager.
4. Drag the selected part onto the part on the schematic page that is to receive the copied properties.

To copy properties from one part to a group of parts, do the following:

1. Open the schematic design that contains the part properties you want to copy.
2. From the Tools menu, point to Part Manager and choose Open. CIS displays the part manager, showing all parts in the design, sorted by part reference.
   
3. In the part manager, select the part with the properties you want to copy.
4. From the Edit menu, choose Copy.
5. Select the destination parts by holding down the Ctrl key while you select individual parts to add to the selected group, or by holding down the Shift key and selecting a contiguous group of parts.
6. From the Edit menu, choose Paste. CIS copies the properties from the first part to all the selected destination parts.

Exporting Variant List to PCB Editor using Part Manager

In Allegro X PCB Editor, you cannot view the assembly drawings for the variants of a design created in Capture CIS. The information about the variants, the part changes for the variants of the design, can be exported to the variants.lst file. Allegro PCB Editor can use this file to import information about the variants. As a result, the variants.lst file serves as a mechanism for passing variant information to Allegro PCB Editor.

To create the variants.lst file, do the following: 

1. From the Tools menu of Part Manager, choose Export Variant List. The Export Variants List dialog box appears.
2. The Output File (Variants.lst) Path field specifies the default location for the variants.lst file.
   The default location is the Allegro folder in the design directory. You can change this path.

Once you are done with creating variants for a design, you can create the variants.lst file in CIS. You can create this file using the Export Variants List dialog box. The variants.lst file can then be imported in the board in PCB Editor.

To create the variants.lst file, CIS needs two inputs:

• Information about the variants of the design. This is obtained from the CIS database.
• Information about the mappings between properties in Capture and those in Allegro PCB Editor. This is given by you in the variant.cfg file.

3. The Config File (Variant.cfg) Path field specifies the default path for the Variant.cfg file.
The default path is the same as that of the Capture.exe file. You can change this path also.

The Variant.cfg File

The mappings between CIS property names and Allegro PCB Editor injected property names are specified in the variant.cfg file. A sample variant.cfg file is located in <install_directory>\tools\capture.

The variant.cfg file contains entries of the following types:

_ <CIS property name> = YES

This means that <CIS property name> has significance in Allegro PCB Editor. It needs to be written into the variants.lst file. A space in the property name is replaced by an underscore. For example, Part Number = YES is written as Part_Number in the variants.lst file.

_ <CIS property name> = NO

This means that <CIS property name> does not have any significance in Allegro PCB Editor. It does not have to be written into the variants.lst file.

_ <CIS property name> = <PCB Editor Property Name>

This means that the equivalent of <CIS property name> in Allegro PCB Editor is < PCB Editor Property Name>. So, the entry in the variants.lst file is made as <PCB Editor Property Name>. For example, PCB Footprint = JEDEC_TYPE is written as JEDEC_TYPE in the variants.lst file.

4. Click Export.
CIS creates a Variant.cfg file containing information about all the variants of the design.

The properties listed are the ones specified in the Variant.cfg file.