The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Modeling >> Semiconductor Devices >> Problem of simkit(NXP) for Cadence installation & simulation
https://designers-guide.org/forum/YaBB.pl?num=1331122330

Message started by Lynn Lou on Mar 7^th, 2012, 4:12am

Title: Problem of simkit(NXP) for Cadence installation & simulation
Post by Lynn Lou on Mar 7^th, 2012, 4:12am

Hi all,
I modelled a RFMOS with PSP model. I got a problem when I install SimKit for Cadence to verify this model with Spectre simulator. After adding model card(*.scs) in ADE Setup->Model Libraries and running simulation , ADE simulation failed and the log suggested as follows:"
ERROR (SFE-395): "/home/psp_model/ModelCard/n12_rf_psp.scs" 84: The primitive 'psp103' could not be found when attempting to create the model 'n12'.
ERROR (SFE-23): "/home/psp_model/ModelCard/n12_rf_psp.scs" 83: n12_psp is an instance of an undefined model n12."

I followed the official instruction when install, but I am not sure whether the installation is success or not.

How can I fix it? Any suggestion will be appreciated~

Title: Re: Problem of simkit(NXP) for Cadence installation & simulation
Post by Geoffrey_Coram on Mar 7^th, 2012, 6:35am

The top of the log file should say something like
Loaded shared object
/path/to/libsimkit.so

if the installation was successful. Also, if you type "spectre -help" at the command line, it should give you a list of available components, and
Components marked with * are loaded from shared objects

Title: Re: Problem of simkit(NXP) for Cadence installation & simulation
Post by Geoffrey_Coram on Mar 7^th, 2012, 6:36am

Also, the most recent versions of Spectre may well have psp103 built in. Are you sure you need the simkit? What version of Spectre are you running?

Title: Re: Problem of simkit(NXP) for Cadence installation & simulation
Post by Lynn Lou on Mar 7^th, 2012, 7:43am

Geoffrey_Coram wrote on Mar 7^th, 2012, 6:35am:

Thank you, Geoffrey_Coram.

In the top of the log, it said "
Cannot access shared object /home/psp_model/libsimkit_spectre_5.0.so.
Cannot access shared object /home/psp_model/libsmk_5.0.so."
Does it mean that the simkit is not intalled successfully? I checked the available components, and PSP102e with * is in the list. How can I use this component?

I am not sure the version of my Spectre, but it is with MMSIM710. Does it have the PSP102/103 built-in?

Plenty of questions...
Thank you very much!

Title: Re: Problem of simkit(NXP) for Cadence installation & simulation
Post by Geoffrey_Coram on Mar 7^th, 2012, 11:29am

Lynn Lou wrote on Mar 7^th, 2012, 7:43am:

In the top of the log, it said "
Cannot access shared object /home/psp_model/libsimkit_spectre_5.0.so.
Cannot access shared object /home/psp_model/libsmk_5.0.so."
Does it mean that the simkit is not intalled successfully?

Indeed, it is not installed. Is that the correct path? Perhaps it should be /home/lynn_lo/psp_model/lib... ?

Quote:

I checked the available components, and PSP102e with * is in the list. How can I use this component?

For any component that's available, you can "spectre -help component" to get more information. Of course, the parameters might not be exactly the same for 102e as 103.

Quote:

I am not sure the version of my Spectre, but it is with MMSIM710. Does it have the PSP102/103 built-in?

That's kind of old. I don't remember the history off the top of my head, but I would guess that 102 is built in but 103 was not released until after MMSIM710.

Title: Re: Problem of simkit(NXP) for Cadence installation & simulation
Post by Lynn Lou on Mar 8^th, 2012, 1:12am

Geoffrey_Coram wrote on Mar 7^th, 2012, 6:36am:

Is that the correct path? Perhaps it should be /home/lynn_lo/psp_model/lib... ?

Sharp deduction, yes, the full path is /home/lynn/psp_model/... . It was not the full path because I deleted some terms to shorten it, but I am sure the path is correct.

I find my Spectre supports psp102e, so I run my model without newly-installed SimKit and netlisting is done successful. But there is not drain current through the NMOS, and log says as :
"Notice from spectre during info `dcOpInfo'.
No outputs were found. Loosening output filter criterion to `lvlpub'.

dcOpInfo: writing operating point information to rawfile.

Notice from spectre during info `modelParameter'.
No outputs were found. Loosening output filter criterion to `lvlpub'.

modelParameter: writing model parameter values to rawfile.
..."

What does it imply? And what shall I do for this?

Thanks for your patience :)

Title: Re: Problem of simkit(NXP) for Cadence installation & simulation
Post by Geoffrey_Coram on Mar 8^th, 2012, 12:11pm

If you're sure the path is correct, I don't know why you'd get "Cannot access shared object" -- is it not readable? I would expect a different message if you'd downloaded the wrong library (eg, the Solaris library instead of linux).

But I guess that's irrelevant now.

Are you running spectre through ADE or at the command-line? I like to run it at the command line, then I can make up a simple netlist with a single psp102e device and two voltage sources (VD, VG) and run a simple dc sweep.

It looks to me like you've got some strange "analysis" that only writes out the model parameters -- it may not actually apply any bias or run any simulation, so that's why there is no current.

Title: Re: Problem of simkit(NXP) for Cadence installation & simulation
Post by Lynn Lou on Mar 8^th, 2012, 10:39pm

Thanks Geoffrey,

Geoffrey_Coram wrote on Mar 8^th, 2012, 12:11pm:

It looks to me like you've got some strange "analysis" that only writes out the model parameters -- it may not actually apply any bias or run any simulation, so that's why there is no current.

I extracted model parameters following PSP manual, maybe some of the parameters I extracted are far from "reality". Now, the model works, although the current is too small than expected. I'd re-check the parameters. The problem "No outputs were found" is caused by my wrong setting in Save Options in ADE.

Geoffrey_Coram wrote on Mar 8^th, 2012, 12:11pm:

I'd try SimKit of latest version later and check the installation flow.

Thank you Geoffrey, for your analysis and advice with patience these days. I really appreciate that.

Title: Re: Problem of simkit(NXP) for Cadence installation & simulation
Post by Geoffrey_Coram on Mar 9^th, 2012, 6:51am

You're welcome.

Also realize that "psp102e" is the "electrical" or "local" model -- there are also "binning" and "global" versions that take scaling rules into account -- and use slightly different parameter names (NSUBO instead of NSUB, perhaps). I think Spectre tells you if you specified a parameter it doesn't recognize and is ignoring -- check your log file.

Title: Re: Problem of simkit(NXP) for Cadence installation & simulation
Post by Lynn Lou on Mar 20^th, 2012, 12:43am

Thanks Geoffrey,

I installed SimKit, and it proved that the installation failed because .cmiconfig file I created in Windows was not recognized by Linux. The SimKit 3.7 supports PSP103, so I switched to PSP103 while simulating afterwards.

Model unconvergence emerge when Trans simulation, and I think some PSP parameters are not properly extracted. Am I right? What else causes convergence problem?

Still on my way :)

Title: Re: Problem of simkit(NXP) for Cadence installation & simulation
Post by Geoffrey_Coram on Mar 20^th, 2012, 7:17am

There are lots of things that can cause convergence problems; Spectre prints out a list of them when it gets stuck. How complicated is your circuit? Have you tried a simple inverter or inverter chain?

Have you looked at dc I-V curves for the device, and do they make sense? Have you looked at C-V curves from ac analysis? Are the body diodes active? (swjuncap>0)

Have you looked at all the warnings from Spectre? Once, I had a problem with inherited connections, such that the body terminal of a MOS device was floating, that caused a convergence issue.

Title: Re: Problem of simkit(NXP) for Cadence installation & simulation
Post by Lynn Lou on Mar 26^th, 2012, 11:29pm

Thanks, Geoffrey,

Geoffrey_Coram wrote on Mar 20^th, 2012, 7:17am:

The circuit is a simple NMOS-based LC VCO, and my model worked well in DC and S-parameter simulation, but failed in Tran simulation.

I can not extract parameters of body diodes since relative data were not available, so I set swjuncap = 0 . Are the diodes critical for convengence?

I checked the device terminals and RF parasitic subcircuit, and I think they were all set. However, I found the non-universality parameter XCOR is significantly affect the convergence. XCOR I extracted is around 3, and model was not convergent in VCO trans sim, but I set XCOR below 1, it converged. Have you ever encounter this circumstance?

Thanks a lot~

Title: Re: Problem of simkit(NXP) for Cadence installation & simulation
Post by Geoffrey_Coram on Mar 27^th, 2012, 7:05am

XCOR appears to be used only in this equation:
Rxcor = (1.0 + 0.2 * XCOR_i * Vsbx) / (1.0 + XCOR_i * Vsbx);

which feeds into the drain saturation voltage. Do you have good measurements for different Vbs values? What do the Vbs values look like in your transient simulation?

Title: Re: Problem of simkit(NXP) for Cadence installation & simulation
Post by Lynn Lou on Mar 28^th, 2012, 12:33am

Thanks Geoffrey,

The sample MOS I have is in GSG test structure with S and B connected to the ground. So the measurement with varied Vbs is not available. Maybe XCOR I extracted was far from reality, and caused convergence problem. Does inappropriate XCOR cause convergence problem?

I am wondering whether the XCOR changes a lot over different process of the same fab. Because I have some data of .13um MOS and I think maybe I can use they to extract XCOR as a reference. Is it practicable?

Thank you~

Title: Re: Problem of simkit(NXP) for Cadence installation & simulation
Post by Geoffrey_Coram on Mar 28^th, 2012, 5:02am

If Vsbx < 0, then the denominator (1.0 + XCOR_i * Vsbx) can cross through zero, and this would certainly give convergence problems.

However, I can't tell from the computations of Vsbx whether it is clamped > 0. (One expects Vsb > 0 normally, so the b-s diode is reverse-biased. However, in switching events, you can get Vsb < 0, but I'm not sure how that affects Vsbx.)

Title: Re: Problem of simkit(NXP) for Cadence installation & simulation
Post by Lynn Lou on Mar 28^th, 2012, 7:49am

I have Terminal S and B connected together while simulating, so theoretically, Vsb<0 will not happen. According to you explanations, Vsb is unavoidable in switching, so the convergence problems occur unless the b-s diode is forward-biased. Am I right? Maybe I should swift onto the junction diode modeling.

Thank you very much :)