Generating Library Parts

Generating a part from a PSpice model library

You can use the Generate Part dialog box to create a part that has pins matching all the hierarchical ports on the root schematic of the design for design reuse. If a destination library file does not exist, Capture creates a library part file (.OLB) that contains the newly generated part and a copy of the top-level schematic. The new .OLB appears in the project manager's Outputs directory along with the new part and schematic. The new part has a reference back to the design where the source schematic resides so that when you descend the hierarchy from the placed part, it will open the source schematic from the destination library.

To generate a part from a PSpice model library

1. From the Tools menu, choose Generate Part to open the Generate Part dialog box.
2. In the Netlist/source file text field, enter the path and name of the file you want to use to generate the part, or click the Browse button to browse for it. Ensure that you change the type of files in the Browse File dialog box to PSpice Model Library Files (*.cir, *.net, *.lib).
3. Select the Implementation name from the drop-down list box in the Implementation options. If more than one model is available, you can choose one from the drop-down list, or you can keep the default setting of <ALL> that appears in the Implementation name and the Part name text boxes. Choosing <ALL> will create a part from all available models.
4. In the Destination part library text field, you can choose to accept the default path and file name, enter the path and name of the file you want to use for the new library, or click the Browse button to search for another one.
5. Click OK.

Generating a part from a schematic or library

You can use the Generate Part dialog box to create a part that has pins matching all the hierarchical ports on the root schematic of a design and use the design as a reuse module.
If a destination library file does not exist, Capture creates a library part file (.OLB) that contains the newly generated part and a copy of the top-level schematic (if the Copy schematic to library option is selected). The new .OLB appears in the project manager Outputs directory along with the new part and schematic. The new part has a reference back to the design where the source schematic resides so that when you descend the hierarchy from the placed part, it will open the source schematic from the destination library.

To generate a part from a schematic design for reuse

1. In the project manager, click to select a schematic folder from which you want to create a part. The schematic can be in a design (.DSN) file or a library (.OLB) file.
   Note: The design file you use for the source must contain ports or the Generate Part operation will fail.
2. From the Tools menu, choose Generate Part. Capture fills in default settings in the Generate Part dialog box.
3. Browse to change the Netlist/source file or keep the default settings. You can generate a part from an external design or from the current design in the active project manager window.
4. Select the Netlist/source file type. For example, choose Capture/Schematic Design if you are generating a design reuse module.
5. Keep the default Part name or enter another name from the design.
   • If the source design has more than one schematic and no schematic is selected, or if more than one schematic is selected, the Part name setting defaults to the root schematic.
   • If the source design is not opened in the current project manager window, its root schematic will be the default Part name.
6. Browse to change the Destination part library or keep the default settings. The default setting creates a new .OLB file that matches the name of the source .DSN file. If the source design is a library (.OLB), the default part library name will be the same name as the source file.
7. Set Primitive property of the new part using the Primitive radio buttons. The default value is No. You can descend from the placed part to its schematic if the Primitive is set to No. For a design reuse module check Default.

8. Select the Copy schematic to library check box if you want to include a copy of the schematic in the new .OLB file along with the new part. This option is unavailable if the source and destination files are the same.

   If you are generating a design reuse module, do not check the Copy schematic to library option. If you do, you will lose occurrence properties that are critical in the design reuse module. Also, checking this option will overwrite the custom library, so make sure to specify an used library name unless you intend to overwrite.

9. Click OK.

To reuse an existing hierarchical design

1. Create a new project or open a working design.
2. In the project manager from the Tools menu, choose Generate Part.
3. Use the Browse button to pick a source design file that has a reusable design and is useful in the working design.
4. Select the schematic to reuse.
5. Enter a resulting library name or keep the default.
6. Select the Copy Schematic to Library Check box and click OK to create a part.
7. Select the schematic page editor window to place instances of the part to reuse its schematic design.
8. Click OK.