Stats

More Content

Import of OpAmp .cir Model in Pspice

MrTF

Hi All,

I tried to import in the PSpice the model of ADA4945 which was downloaded through the AD website.

The model contains several .Subckt which I cannot really understand how are these utilized by the PSpice Simulation Engine.

I was not able also to find a step by step guide to import that model "properly" in the Capture.

I did used though the PSpice model editor to open the file.cir, generate an .olb file and then modify the schematic symbol through the Capture.

Afterwards I created a new project where I was able to place the component but I encountered the following error.

ERROR(ORPSIM-15108): Subcircuit ADA4945 used by X_U1 is undefined.

Any clues about what this error is related to and how I can eliminate it?

After interrating the process of importing the model as described in the Annex C of the Pspice User guide I came up with the following errors:

ERROR(ORPSIM-16362): Name on .ENDS does not match .SUBCKT

ERROR(ORPSIM-15113): Model Res1 used by X_U1.Rv1 is undefined

ERROR(ORPSIM-15113): Model Res2 used by X_U1.Rv2 is undefined

ERROR(ORPSIM-15113): Model Res3 used by X_U1.Ros1 is undefined

ERROR(ORPSIM-15113): Model Res4 used by X_U1.Ros2 is undefined

ERROR(ORPSIM-15113): Model Res5 used by X_U1.RbP1 is undefined

ERROR(ORPSIM-15113): Model Res6 used by X_U1.RbN1 is undefined

ERROR(ORPSIM-15108): Subcircuit ADA4945-H-Amp used by X_U1.X1H is undefined

ERROR(ORPSIM-15108): Subcircuit ADA4945-H-Amp used by X_U1.X2H is undefined

ERROR(ORPSIM-15108): Subcircuit ADA4945-H-Vocm used by X_U1.X3H is undefined

ERROR(ORPSIM-15108): Subcircuit ADA4945-L-Amp used by X_U1.X1L is undefined

ERROR(ORPSIM-15108): Subcircuit ADA4945-L-Amp used by X_U1.X2L is undefined

ERROR(ORPSIM-15108): Subcircuit ADA4945-L-Vocm used by X_U1.X3L is undefined

  • 0

    The original CIR file has some issues as far a PSpice is concerned. If a .ENDS statement has any text following on the same line, that text must match the name of the .SUBCKT. So, an opening subcircuit with .SUBCKT ABC123 ... must have a .ENDS ABC123 at the close of the subcircuit, anything else will be an error as far as the Model Editor is concerned. A .ENDS alone is always accepted so, in this case, edit the CIR file with a plain text editor, like Notepad, and change all of the .ENDS lines that have any following text to just be .ENDS and the Model Editor will accept the file - rename the modified file to be a .LIB and the Model Editor will open it without needing to change the "Files of Type". You will then get all of the subcircuits in the file and you can create the Capture parts. You will need to add the OLB file to the schematic part libraries to place the part and also add the saved LIB file to Configuration>Libraries in the PSpice Simulation Profile to get the model found when the simulation runs, using Add to Design is the preferred option.

  • +1

    test_AD4945-2023-12-14T14-07.zip

    The other issue is that the intrinsic resistor model for PSpice is RES, not R. This model seems to use both. The attached project archive runs a simulation of a circuit based on an extract of a sample test circuit on the AD site for the part. The .ENDS and R / RES issues have been addressed in the model and allow the simulation to run. Note that there are some messages related to negative resistance being evaluated due to temperature coefficients when the simulation runs and the use of "Rmin" in these cases may have some impact on the results.

  • 0 in reply to oldmouldy

    Thanks for your effort in correcting those subcircuits and preparing a simulation of the ADA4945 model.  I ran it and saw the negative resistance messages.  The TNOM entries in the parameter fields of the six Res models bothered me as they didn't fit the PSpice syntax.  I removed them and ran your simulation again and didn't see those messages.  The header of the .cir file states that this model has been tested on LTSPice, MultSIm, SiMetrix(NGSpice), and PSpice so maybe they were just remnants of that work and needed to be removed for use with PSpice.

Cadence Guidelines

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.