The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> Monte Carlo simulation with HSpice
https://designers-guide.org/forum/YaBB.pl?num=1141226185

Message started by vincent on Mar 1^st, 2006, 7:16am

Title: Monte Carlo simulation with HSpice
Post by vincent on Mar 1^st, 2006, 7:16am

Hi,

I have simulated a netlist with two resistors in serie with HSpice 2003 and HSpice 2005. That was Monte carlo simulation for mismatch.
The model is built in the same way as in the documentation "Recommended Spectre Monte Carlo modeling methodology".
There is no problem with HSpice 2003 but for the version of 2005 we don't see the mismatch between the both resistors.

**Libraries HSPICE**
.lib 'libraries' include_file
*.lib 'share/hspice/process.h' process_variations
*.lib 'share/hspice/process.h' process_mismatch_variations
.lib 'share/hspice/process.h' mismatch_variations
.lib 'libraries' include_model

**Analyse statements**
vamp1 input drain 0

***Mapping Resistors***
*---R11---
vd input 0 +10
vsubr1 subr1 0 0
vsubr2 subr2 0 0

***Devices Under Test (DUT)***
*--RESISTORS--
Xr1 drain probe subr1 R11 R=10K W=0.77u
Xr2 probe 0 subr2 R11 R=10K W=0.77u

****Extraction statements****
.option seed=1
.OP
.print DC I(vamp?)
.print DC V(input)
.print DC V(probe)

**Launch of the simulation**
********MONTE-CARLO*********
.DC MONTE= 20

.END

Is there any main differences between the version 2003 and the version 2005 of HSpice concerning the mismatch simulation?
I hope you will understand my question.

Second question: I have the same problem between Spectre alone and Spectremdl. Spectre works correctly.
Thanks

Title: Re: Monte Carlo simulation with HSpice
Post by Geoffrey_Coram on Mar 3^rd, 2006, 4:44am

If there's a difference between versions of HSpice, you should probably check with your applications engineer/support person. Sounds like it could be a bug in HSpice 2005 -- or maybe they changed the setup so you have to set a .option card to get it to work in 2005. (Seems a little hard to believe that they would have "accidentally" disabled Monte-Carlo ...)

Title: Re: Monte Carlo simulation with HSpice
Post by KristinBeggs on Mar 3^rd, 2006, 5:17am

Vincent,

It would also be good to see the process.h file. You state that the model is built according to the "Recommended Spectre" methodology. Does the process.h file include a statistics/process block? Or are the statistical distribution functions found in the parameters statements themselves?

Kristin

Title: Re: Monte Carlo simulation with HSpice
Post by vincent on Mar 3^rd, 2006, 6:18am

That is still me

In fact the problem is the following: I can see my mismatch distributions in my output file BUT I had expceted that HSpice would have taken a new random for each instance of a resistor, and that is not the case for the new version HSpice 2005.
Concerning the process.h file, it contains the distribution with a syntax like : + rsh_r11_mm= agauss(0, 1, 1)
rsh for sheet resistance , mm for mismatch
and this parameter is then multiplicated by the sigma in the model (that is a subcircuit) to find the whole distribution.
The process.h file contains also process deviations but in others sections which are not chosen in the netlist.

It should be a problem with a new way of choosing the random number in the monte carlo simulation.
Remark: I use the same files with HPsice 2003 and HSpice 2005

Thanks

Title: Re: Monte Carlo simulation with HSpice
Post by Scott Flinchbaugh on Mar 10^th, 2006, 11:54am

Vincent,

There was an issue with spectremdl and montecarlo mismatch variations.

The next ISR of mmsim6.0 fixes the problem. It should be available the
end of march.

Best Regards,
-scott

Title: Re: Monte Carlo simulation with HSpice
Post by Geoffrey_Coram on Mar 15^th, 2006, 5:30am

Scott -
Vincent's message was talking about problems in HSpice. (Thanks for telling us about an issue in Spectre, in case that comes up for someone else ...)

Title: Re: Monte Carlo simulation with HSpice
Post by spiceoracle on May 31^st, 2006, 2:57pm

You didn't mention which 2005 version you are using but, from your description, I suspect that you are using the 2005.09 version. If so, there was a bug in this version that affects Monte Carlo simulations when the parameters are defined within subcircuits. This bug has been fixed in the 2006.03 release.

Title: Re: Monte Carlo simulation with HSpice
Post by vincent on Jun 8^th, 2006, 1:07am

Thank you very much. That was effectively the case: I used the version 2005.09. But I could have used eldo and spectre to simulate what I wanted.

Vincent