Convergence issue in PSpice with many OPA models

Etienne,

Without seeing the circuits, its hard to make any recommendations beyond using Pspice's advanced convergence features.
The models may be contributing factors, but so could the initial conditions, the circuits' operating points, the simulation waveforms and the circuits themselves.

Can you upload the Pspice projects to this thread and we will see if we can improve their convergence?

Please note that we have an online filter design and simulation tool - WEBENCH Filter Designer. 
You can design active filters, generate the circuit BOMs, and simulate the final circuit.
 It is available at ti.com:

http://www.ti.com/lsds/ti/analog/webench/overview.page

Go to the URL & press the Filter tab to get started.

Regards,
John

Hello John,

Thanks for your quick answer.
It's the first time I'm using this forum, how can I upload or attach a design in a thread?

In between, here is the netlist:
* source ACTIVE_FILTER
V_V1 VCC 0 3Vdc
C_C2 N00925 N00703 330p IC=0 TC=0,0
R_R1 N00469 OUT 130k TC=0,0
R_R2 N00383 OUT_FILT 130k TC=0,0
R_R3 N00703 N00383 10k TC=0,0
R_R4 N00925 N00469 10k TC=0,0
R_R5 N00736 N00439 39k TC=0,0
R_R6 N00736 N00473 39k TC=0,0
C_C3 0 OUT 1p TC=0,0
C_C4 0 OUT_FILT 1p TC=0,0
V_V2 N00736 0 1.5Vdc
V_V3 N00925 N00736 AC 1
+SIN 0 1m 50k 0 0 0
C_C5 N00383 OUT_FILT 22p TC=0,0
X_U1 N00473 N00469 VCC 0 OUT OPA348
X_U2 N00439 N00383 VCC 0 OUT_FILT OPA348

Regards,
Etienne

Sorry, in fact it's quite easy to upload a bench :-)

Here is my bench with the OPA316:

* Local Libraries :
.LIB "U:/models/opamp/OPA316.lib"
* From [PSPICE NETLIST] section of C:\Users\xxx\AppData\Roaming\SPB_Data\cdssetup\OrCAD_PSpice/16.6.0/PSpice.ini file:
.lib "nom.lib"

*Analysis directives:
.AC DEC 25 10 1meg
.NOISE v([OUT_FILT]) V_V3 10
.OPTIONS ADVCONV
.PROBE64 V(alias(*)) I(alias(*)) W(alias(*)) D(alias(*)) NOISE(alias(*))
.INC "..\SCHEMATIC1.net"



**** INCLUDING SCHEMATIC1.net ****
* source ACTIVE_FILTER
V_V1         VCC 0 3Vdc
C_C2         N00925 N00703  330p IC=0 TC=0,0
R_R1         N00469 OUT  130k TC=0,0
R_R2         N00383 OUT_FILT  130k TC=0,0
R_R3         N00703 N00383  10k TC=0,0
R_R4         N00925 N00469  10k TC=0,0
R_R5         N00736 N00439  39k TC=0,0
R_R6         N00736 N00473  39k TC=0,0
C_C3         0 OUT  1p  TC=0,0
C_C4         0 OUT_FILT  1p  TC=0,0
V_V2         N00736 0 1.5Vdc
V_V3         N00925 N00736  AC 1
+SIN 0 1m 50k 0 0 0
C_C5         N00383 OUT_FILT  22p  TC=0,0
X_U1         N00473 N00469 VCC 0 OUT OPA316
X_U2         N00439 N00383 VCC 0 OUT_FILT OPA316

**** RESUMING ac.cir ****
.END

I plot the following signals: DB(V(out)), DB(V(out_filt)), DB(V(ONOISE))

The center frequency of my band-pass filter is 50kHz where I should have a gain of about 17dB, but with the OPA316, it take a while to converge and the output AC is completely wrong. I also see a current of about 3.5uA at amp input which is completely wrong as the data sheet tell is +/- 15nA over temperature range.

Regards,

Etienne

Etienne,

Thank you.

Please note that you can upload the zipped Cadence project files by pressing the paper clip icon on the command bar just above the message text box.

If you can do this, we can work at the schematic level. That will hopefully speed up getting your problem resolved.

Regards,
John

Hello John,

Find attached my test benches.

Here are my inputs about the 5 different benches I sent:

OPA313: unsimulable, it's look like there is an error in the model. The simulator give the following message: "ERROR(ORPSIM-15143): Voltage source and/or inductor loop involving X_U1.XU7.VSENSE. You may break the loop by adding a series resistance"
OPA376: Work fine.
OPA348: Don't always give the same result. For exemple, yesterday the BW of the amp was around 300kHz and the peak of my band-pass was under 30kHz
OPA316: Take a while to find convergence (107s), wrong results, input bias current up to 3.5uA, strange bias point.
All amp together: Conflict between models. I was able to remove some error message by renaming some subckt in different models, but still wasn't able to simulated due to the error in the OPA313 model.

I also see that the OPA348 doesn't converge if simulated with a non-ideal supply. I didn't try with others.

Regards,

Etienne

OrCAD_test.zip

Etienne,

I was able to correct the OPA313 model so it doesn't give a Pspice error.
It is in the models folder in the attached project file. The original model was optimized to work in TINA, a free circuit simulator we offer.
Apparently TINA is okay with the model as-is, but Pspice objected to some of the internal connections.
In the revised model, one of the internal nodes was split into two new nodes using a 1p0hm resistor. It seems to be okay now.

I didn't see any convergence problems with the other single devices. They seemed to work fine.

One thing that seemed important was to be sure the Advanced Convergence box was checked in the Sim Settings/Options panel.

There were some conflicts in the all test bench because of subcircuit names that are shared between the models.
That has been corrected in the  attached models library.
The test bench seems to run now, but the bias points seem to be off compared to the single-circuit results. It will take some experimentation with the accuracy-related sim parameters.

Please let me know if you have any more questions.

Regards,
John

OrCAD_test_rev.zip

John,

Thanks you very much for your investigation!

Now the OPA 313 work and give correct results. Even it take 110s to converge.

I take a look at your .out files of the OPA313 and OPA316, and it's just amazing. For you, both OPA does simulate in less than a second and give correct results, and by me, both amp take more than 100s to converge and the OPA316 give a completely wrong results.

I use the default options of the simulator, which looks the same as yours. Comparison between our .out files, advanced convergence is enable in both case.

Which version of OrCAD does you use? I'm currently using the version 16.6-S053.

Regards,

Etienne

Etienne,
I am using Cadence version 16.6 S027.
A colleague suggested some things to look at, so the investigation is still in progress. I will give an update later today or Monday.
Regards,
John

Hello John,

Thanks for your investigation. I also send my test bench to the Cadence support and they experience the same issue as me: long convergence time and wrong results. They are asking about your OrCAD version details like the picture here under. In PSpice --> Help --> about PSpice --> version info. They also ask if it would be possible to give us your pspice.ini file?

Thanks in advance.

Best regards

Etienne

Etienne,

The version info is below. Pspice is the simulation engine behind Allegro.

Apologies Etienne. Our system removed the images in my last reply.

The version info should show up this time.
The tool is Allegro, and it uses Pspice as the sim engine.