PSpice generated file in OrCAD Capture

In Capture there are bias points you can enable, and voltage, current and power markers that you can add. Otherwise, when the simulation ends, use trace>add trace to get the waveforms in the probe window. (Menu for Markers, PSpice>Markers, pick marker, for Bias Points, PSpice>Bias Points, enable the Bias Point display, bias points are displayed in the schematic - or use the toolbar icons)

oldmouldy said:

In Capture there are bias points you can enable, and voltage, current and power markers that you can add. Otherwise, when the simulation ends, use trace>add trace to get the waveforms in the probe window. (Menu for Markers, PSpice>Markers, pick marker, for Bias Points, PSpice>Bias Points, enable the Bias Point display, bias points are displayed in the schematic - or use the toolbar icons)

Yes, I can use add a trace, but I was saving that for my next question (Steady state DC doesn't need a time trace, and it is giving a trace of voltage vs voltage, which I'm not clear as to what it's trying to show me).

Since this is just a simple steady state circuit, I am trying to get the node data in the output file from the .PRINT command, like this:
  Is          V(Ra)       V(Rb)       V(Rc)       V(2)        V(3)        
   4.000E+00   1.200E+02   1.000E+02   5.000E+02   5.000E+02   7.200E+02
I can't place a cursor on the graph to see the exact value because it complains there is no valid trace.

This is what I am trying to figure out.

Thanks.

-Scotty

The Probe WIndow won't display anything for the Bias simulation since this is a simple steady state with nothing changing. View the Output File, this will list the node voltages at the start of the simulation, actually the end for a Bias Simulation. In Capture, you can also turn on the Bias Markers and have the initial steady state values displayed on the schematic.

Thanks for your response. However, that's not getting me any closer.

 I *really* wish there was a better tutorial...

I have been examining the *.out file, the node values aren't in it, because the *.cir  and/or *.net files don't have a .PRINT command.
I did manage to decypher the structure that was being used (profile file name is the *.cir file, which includes the *.net files for each drawing).  Aparently, the 'Analysis Directives' section of the *.cir file is where the .PRINT command should be placed, I just can't figure out how to get the Capture program to place it there.  All the files have big statements that say
** Creating circuit file "Test.cir"
** WARNING: THIS AUTOMATICALLY GENERATED FILE MAY BE OVERWRITTEN BY SUBSEQUENT SIMULATIONS
So, I can't put the .PRINT command in manually.

Since I can't see how to attach a file, here is a paste of the *.out file.  There are no node voltages in it.  Remember, this is a tiny little two mesh loop, just to try to learn the suite, not solve some hugh complex problem.

Thanks for your continued help.

 ----------------------------------PASTE--------------------------------------------------------
**** 01/16/09 09:40:16 ******* PSpice Lite (August 2007) ****** ID# 10813 ****

 ** Profile: "Mesh1-Test"  [ C:\Demo\Meshes\mesh-pspicefiles\mesh1\test.sim ]

 ****     CIRCUIT DESCRIPTION

******************************************************************************

** Creating circuit file "Test.cir"
** WARNING: THIS AUTOMATICALLY GENERATED FILE MAY BE OVERWRITTEN BY SUBSEQUENT SIMULATIONS

*Libraries:
* Profile Libraries :
* Local Libraries :
* From [PSPICE NETLIST] section of C:\OrCAD\OrCAD_16.0_Demo\tools\PSpice\PSpice.ini file:
.lib "nom.lib"

*Analysis directives:
.DC LIN V_V1 12 12 1
.PROBE V(alias(*)) I(alias(*)) W(alias(*)) D(alias(*)) NOISE(alias(*))
.INC "..\Mesh1.net"

**** INCLUDING Mesh1.net ****
* source MESH
R_R1         N00223 N00196  5k 
R_R2         N00196 N00187  500 
R_R3         0 N00196  1k 
V_V1         N00223 0 12Vdc
I_I2         0 N00187 DC 15mAdc 

**** RESUMING Test.cir ****
.END

          JOB CONCLUDED

**** 01/16/09 09:40:16 ******* PSpice Lite (August 2007) ****** ID# 10813 ****

 ** Profile: "Mesh1-Test"  [ C:\Demo\Meshes\mesh-pspicefiles\mesh1\test.sim ]

 ****     JOB STATISTICS SUMMARY

******************************************************************************

  Total job time (using Solver 1)   =        0.00

Check the Simulation Profile, PSpice>Edit Simulation Profile, on the Analysis tab, you cleared the default flag to "include detailed bias point information for nonlinear controlled sources and semiconductors (.OP)", this does not affect the output file but it does indicate that the simulation profile has been changed and the reason that you are not getting any bias values in the output file. On the Options tab, change the category to "Output File" and check the box to include "Bias Point Node voltages" in the output file, the Bias Points will then be listed in the output file. The fact still remains that the display of bias points can be enabled in the schematic.

Yes. That did it. Thanks.

The values are showing up in the *.out file.  And the bias 'pins' on the schematic have results too.  (Bias Point Node Voltages was already turned on, I guess the change to the profile was what was needed).