This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

opa694 pspice macromodel

Other Parts Discussed in Thread: OPA694

Hi, my name is Sarah, I am currently doing a class project to simulate different configurations of instrumentation amplifiers using Cadence and Pspice
I would like to compare different opamps responses but i'm a beginner with Pspice files and i don't manage to use the macromodel of the OPA694, having always the same errors appearing:

X_U1.F3 X_U1.28 X_U1.29 X_U1.VC Zo
ERROR(ORPSIM-16152): Invalid number

X_U1.F4 X_U1.32 X_U1.33 Zo
ERROR(ORPSIM-16047): Must be V

 I am really interested in making the simulation work to compare with my physical circuit as i got satisfying results with this CFA.

THanks in advance for your help, 


  • Sarah,

    I am a modeling engineer in the WEBENCH Design Center.

    I will try to find the source of the error message and have a fix by close of business tomorrow.



  • Sarah,

    Checking the OPA694 model netlist, it appears  the lines for subcircuit calls in the main netlist must be commented or uncommented depending on the simulator being used. Has that been taken into account?

    For example, the subciruit call for OPA694_F1 just below has some instructions:

    .SUBCKT OPA694 + - Out V+ V-
    I_I1         20 21 DC 1.24mA 
    X_F1    19 20 24 25 OPA694_F1       *comment out when using with 3F4
    *F1   19 20 24 25 1.0               *comment out when used PSpice

    It looks like the default comment/uncomment state for the subcircuit calls is for Pspice, at least for the version I downloaded from

    Please take a look at your model file and let me know what you find.
    It it looks okay, then please upload your Pspice project and we can try to diagnose what's going on.



  • Dear Mr Miller,

    Thank you very much for helping me and for your reactivity, I really appreciate.
    Though i took into account the comment/uncomment lines following the instructions before i asked you for your help.
    I thought the problem could come from "Zo" as it appears in all the error lines, but i can't find out why.
    I'm using the 16.3 and 16.5 versions of Cadence in case if this information can be relevant. 
    I used the model provided by and generated the files .lib and .olb with the "Model Editor".
    My project for now looks like any instrumentation amplifier, using 3 opamps (preferibly current-feedback)

    Once again, i'm really grateful for your help and your time, hoping i/you/we can make this model work.

    Best regards,


  • Sarah,

    After some investigation, it appears part of the problem are the comments that follow the active lines in the netlist.

    For example, just after the main subcircuit definition there are some in-line comments:
    .SUBCKT OPA694 + - Out V+ V-
    I_I1         20 21 DC 1.24mA 
    X_F1    19 20 24 25 OPA694_F1       *comment out when using with 3F4
    *F1   19 20 24 25 1.0               *comment out when used PSpice

    The comment on the *F1 line isn't a problem, but the comment on the X_F1 line seemed to confuse Pspice.

    Placing the comments on a new line just above statetments seemed to eliminate those errors.
    SUBCKT OPA694 + - Out V+ V-
    I_I1         20 21 DC 1.24mA 
    *comment out when using with 3F4
    X_F1    19 20 24 25 OPA694_F1      
    *comment out when used PSpice
    *F1   19 20 24 25 1.0

    This change was done for all of the comments that share a line, even with the subcircuit statements near the bottom of the netlist.

    One of the E-source statements had some missing spaces.
    The line:

    E_E1         36 0 POLY(1) V+ V-  -.1.25  .5  0 
    has a problem because there are too many decimal points in one of the numbers.
    Changing it to the following eliminated the errors:
    E_E1         36 0 POLY(1) V+ V-  -0.1 0.25  0.5  0

    The modified netlist file is attached to this thread.

    Hope this helps.

    Please let me know if you have any questions.



  • Dear Mr Miller,

    I used the file you sent me with the modifications you made and it seems to work this time, no errors and the simulation runs!!
    I am sincerely grateful that you helped me that rapidly solving this problem.
    If there is some way to rate customer's satisfaction, you can add a ++ from me!

    Kind regards,