Designer’s Guide Community

vincent

New Member

Offline

Posts: 3

Monte Carlo simulation with HSpice
Mar 01^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

Back to top

IP Logged

Geoffrey_Coram

Senior Fellow

Offline

Posts: 1999
Massachusetts, USA

Re: Monte Carlo simulation with HSpice
Reply #1 - 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 ...)

Back to top

If at first you do succeed, STOP, raise your standards, and stop wasting your time.

IP Logged

KristinBeggs New Member Offline Posts: 2	Re: Monte Carlo simulation with HSpice Reply #2 - 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
Back to top	IP Logged

vincent

New Member

Offline

Posts: 3

Re: Monte Carlo simulation with HSpice
Reply #3 - 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

Back to top

IP Logged

Scott Flinchbaugh Junior Member Offline Posts: 14	Re: Monte Carlo simulation with HSpice Reply #4 - 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
Back to top	IP Logged

Geoffrey_Coram Senior Fellow Offline Posts: 1999 Massachusetts, USA	Re: Monte Carlo simulation with HSpice Reply #5 - 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 ...)
Back to top	If at first you do succeed, STOP, raise your standards, and stop wasting your time. IP Logged

spiceoracle Junior Member Offline Posts: 21 USA	Re: Monte Carlo simulation with HSpice Reply #6 - 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.
Back to top	IP Logged

vincent New Member Offline Posts: 3	Re: Monte Carlo simulation with HSpice Reply #7 - 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
Back to top	IP Logged