The application notes presented in the instructions that follow describe how you can create a SPICE model you find on the Internet (such as an op-amp) and tie it to a permanent schematic library part that you can then place in a working design. 

These instructions assume a suitable schematic library part can be found or has already been created.

The instructions that follow use v17.2 hotfix017 of the OrCAD software.


  1.  Make or get the PSpice .lib file:  
    1. Browse to the Internet and find the text for the model that you want to use.

    2. Copy and paste the text into a text editor.

    3. Save the file as a .lib file using the format: filename.lib.
      You may name the file as desired, but the file extension must be .lib.

  2.  Create a Capture Symbol (.olb):
    1. Open PSpice Model Editor (Start > All Programs > Cadence Release 17.2-2016 > Product Utilities > PSpice Utilities > Model Editor).

    2. Go to File > Model Import Wizard

    3. Browse for the .lib file you created in step 1c. 
      1. The destination directory automatically populates. However, you may change the directory path as desired.
      2. Click Next >. 

    4. Fine the PSpice model that you want to attach to a custom symbol from the list. Next to the symbol there may or may not be a symbol name. Select that box and click Associate Symbol to browse for an existing Capture symbol to use as a copy of this this PSpice model.


    5. Browse for the symbol you want to view.

      Note: The location of PSpice default *.olb libraries is:
      <install>\tools\capture\library\pspice\ <default installation> is C:\Cadence\SPB_17.2

    6. Pick the library and then the resulting list of parts will show the parts with the same number of pins. Choose one that you’d like to use as a template symbol for your PSpice model - click Next >  

    7. Match the PSpice library input names to the symbol names.

      While it may often be easy to map the symbol names to the model names, occasionally mapping symbol names to model names may be more difficult. If this is the case click View Model (lower left hand corner) and usually at the top of the PSpice model file, it has a list of how things get connected.


    8. Click Save Symbol and then Finish. The (*.old) OrCAD Model Library is saved for you.

    9. Close the PSpice Model Editor.

  3. Place your graphic symbol in Capture.

    1. Open OrCAD Capture (Start > All Programs > Cadence Release 17.2-2016 > OrCAD Capture or OrCAD Capture CIS).

    2. Open a design that you want to use for placement of the new PSpice part. This design must be a PSpice analog or mixed A/D design.


    3. Open where you want to place the part.

    4. Go to Place >Part and add a library (in the Libraries space choose the dotted rectangle icon).


    5. Browse for the .olb file that you made in step 2h.  

    6. Place the part in your design.

  4. Configure PSpce .lib file for use with Capture.  

    1. Select PSpice > Edit Simulation Profile > Configuration Files Tab > Library Category from Capture.   
    2. Select the Browse button that is next to Filename and navigate to the .lib file you created in step 1c.


    3. Choose either Add as Global / Add to Design / Add to Profile to choose a location where your .lib file will be available.