I created a Pspice part using the Spice file provided by TI. When simulating, I get the following error:

ERROR(ORPSIM-15108): Subcircuit RNOISE_FREE_0 used by X_U1.XR101 is undefined ERROR(ORPSIM-15108): Subcircuit RNOISE_FREE_0 used by X_U1.XR105 is undefined ERROR(ORPSIM-15108): Subcircuit RNOISE_FREE_2 used by X_U1.XR104 is undefined ERROR(ORPSIM-15108): Subcircuit RNOISE_FREE_0 used by X_U1.XR103 is undefined

Some of the lines with the offending subcircuits are as follows:

XR109_3 23 9 RNOISE_FREE_0 XR109_4 41 9 RNOISE_FREE_0

Would 'RNOISE_FREE...' be circuits recognized by TINA (TI's software) but not by PSPICE? Could I replace them with an equivalent?


  • \$\begingroup\$ Have you added the new .lib file in the Simulation Settings dialog? \$\endgroup\$ Commented Jan 13, 2015 at 4:04
  • \$\begingroup\$ It might also help to tell us which version of PSPICE you're using. \$\endgroup\$ Commented Jan 13, 2015 at 16:07

2 Answers 2


Yes, I have faced similar problem while executing one of my simulation circuits using opa4132.lib file. I have copied all files related to OPA4132 to PSpice library but it did not help. So then in simulation settings, I have changed some limits value like (ABSTOL) and (ITL1) but still the same result.

Finally, I have done something which really helped me to solve this issue. You can try these steps:

  1. In EDIT SIMULATION PROFILE window select "Configuration Files" menu
  2. On left side when you select "Library" option, you can see one file named nom.lib. Here you need to add your .lib file. In my case it was OPA4132.
  3. To do that go to browse option, in that select required .lib file and then click on "Add to Design" menu. Then click on OK.
  4. Now you execute your simulation.

Hope it will work.


I think you have copied only the OPA188 subcircuit (.SUBCKT OPA188 ... till the nearest .ENDS statement) out of the OPA188.lib file provided by Texas Instruments. Am I right? Or what have you exactly done with the OPA188.lib file while making your own library item concerning this part?

Copying only the OPA188 subcircuit, however, is not enough!

There are a few other (nested) subcircuits defined in this library file, among them .SUBCKT RNOISE_FREE_0, .SUBCKT RNOISE_FREE_2, etc., that are used (called) within the main .SUBCKT OPA188 during simulation. You have to use the whole "code" part of the OPA188.lib file (copy it into "your" library).

The error message usually contains only a few first errors occurred after start of simulation, that's why the report doesn't contain all missing subcircuits (I'm sure there are more missing than those two there).


Not the answer you're looking for? Browse other questions tagged or ask your own question.