Designer’s Guide Community

Pavel Senior Member Offline Posts: 174 Lausanne/Switzerland	using Eldo models in Spectre? May 07^th, 2007, 3:15am Hello, How can I use Eldo models in Spectre simulator? Is there some conversion program/script? Regards Pavel.
Back to top	IP Logged

Andrew Beckett

Senior Fellow

Offline

Life, don't talk to
me about Life...

Posts: 1742
Bracknell, UK

Re: using Eldo models in Spectre?
Reply #1 - May 7^th, 2007, 4:18am

Pavel,

For the most part, they should work as is. spectre can read native SPICE models and usually would be able to read model files with no trouble.

Have you tried that? Just make sure that the file does not have a ".scs" suffix (otherwise that tells spectre to read it in spectre syntax) and include the file. Make sure you're using an MMSIM version (preferrably MMSIM61, since MMSIM60 is no longer supported).

Best Regards,

Andrew.

Back to top

IP Logged

Pavel

Senior Member

Offline

Posts: 174
Lausanne/Switzerland

Re: using Eldo models in Spectre?
Reply #2 - May 7^th, 2007, 7:06am

Andrew,

First, thank you for rapid answer.
Yes, I already tried it. I choosed Spectre as simulator and put +csfc option to force Spice syntax recognition.
But it was not sufficient. In Eldo model there are functions (for example trunc) that are not recognized by Spectre parser.
Moreover Eldo model of nmos/pmos contains directive Level=60. I searched for level 60 in Spectre Reference manual, but without success.

Regards,

Pavel.

P.S. What is MMSIM and where can I find its version?

Back to top

IP Logged

Geoffrey_Coram Senior Fellow Offline Posts: 1999 Massachusetts, USA	Re: using Eldo models in Spectre? Reply #3 - May 7^th, 2007, 8:18am Every simulator has its own LEVEL system. Do you know if level=60 in Eldo is supposed to be BSIM3, BSIM4, or something else? I think these are level=49 and =54 respectively in "spice." One can generally deduce the model by looking at the parameters that are specified, if one doesn't have the (Eldo) user's guide.
Back to top	If at first you do succeed, STOP, raise your standards, and stop wasting your time. IP Logged

Pavel

Senior Member

Offline

Posts: 174
Lausanne/Switzerland

Re: using Eldo models in Spectre?
Reply #4 - May 8^th, 2007, 5:00am

Geoffrey,

First, thank you for response.
I compared liste of parameters of BSIM4 Spectre level 14 (from manual) with BSIM4 Eldo level 60 (form model from our Design Kit). There are quite a lot of differencies.

As number of parameters is huge (about 300), it's rather difficult (or time consumming) to establish correspondance.

Apart from this I've found in Design Kit file with extension .so, that sounds like model library. What is this file and can I use it?

I've noted that when I run simulation in ADE, first 5 lines in log window are:

Loading /mnt/ed/cadtools/lic5141_USR2.3/tools.lnx86/cmi/lib/4.0/libinfineon_sh.so
� � � �...
Loading /mnt/ed/cadtools/lic5141_USR2.3/tools.lnx86/cmi/lib/4.0/libnortel_sh.so
� � � �...
Loading /mnt/ed/cadtools/lic5141_USR2.3/tools.lnx86/cmi/lib/4.0/libphilips_sh.so
� � � �...
Loading /mnt/ed/cadtools/lic5141_USR2.3/tools.lnx86/cmi/lib/4.0/libsparam_sh.so
� � � �...
Loading /mnt/ed/cadtools/lic5141_USR2.3/tools.lnx86/cmi/lib/4.0/libstmodels_sh.so

What this information means?

Regards

Pavel

Back to top

IP Logged

Geoffrey_Coram

Senior Fellow

Offline

Posts: 1999
Massachusetts, USA

Re: using Eldo models in Spectre?
Reply #5 - May 8^th, 2007, 5:54am

Pavel wrote on May 8^th, 2007, 5:00am:

I compared liste of parameters of BSIM4 Spectre level 14 (from manual) with BSIM4 Eldo level 60 (form model from our Design Kit). There are quite a lot of differencies.

That surprises me. I know every simulator adds a few special flags, but it should be just a few.

Quote:

As number of parameters is huge (about 300), it's rather difficult (or time consumming) to establish correspondance.

Spectre is "nice enough" to ignore any parameters it doesn't know, so if you just change level=60 to level=14 you should be able to run it and see which one Spectre says it doesn't know (rather than checking all 300 individually). You might also want to check the version= value; the default is not the latest, and it may ignore new parameters from the latest version if you don't set the version correctly.

Quote:

Apart from this I've found in Design Kit file with extension .so, that sounds like model library. What is this file and can I use it?

.so is a "shared object" -- similar to a DLL in Windows. Eg, the libphilips_sh.so contains the Mextram and PSP transistor models.

Back to top

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

IP Logged

Pavel

Senior Member

Offline

Posts: 174
Lausanne/Switzerland

Re: using Eldo models in Spectre?
Reply #6 - May 9^th, 2007, 1:25am

Geoffrey,

Quote:

so if you just change level=60 to level=14 you should be able to run it and see which one Spectre says it doesn't know

Thank you fot hint. I tried it. For the moment I've problem with model syntax.

At the begining of Eldo model there is following piece of code

Code:

.SUBCKT ENULLMM9JU D G S B
+ � � � param: W=10e-6 L=10e-6 nfing=1 mismatch=1 srcefirst=1
+ � � � wfing={w/nfing+3.6e-08}
+ � � � fd={srcefirst*(nfing-2*trunc(nfing/2))+(1-srcefirst)*(2*trunc(1+nfing/2)-nfing)}
+ � � � fs={2-fd}
+ � � � AD={wfing*(nfing*(5.2e-07-(-2.8e-08))/2+fd*(1.4e-07+(3.6e-08)/2))}
+ � � � AS={wfing*(nfing*(5.2e-07-(-2.8e-08))/2+fs*(1.4e-07+(3.6e-08)/2))}
+ � � � PD={nfing*2*(5.2e-07-(-2.8e-08))/2+fd*(wfing+2*1.4e-07+(3.6e-08))}
+ � � � PS={nfing*2*(5.2e-07-(-2.8e-08))/2+fs*(wfing+2*1.4e-07+(3.6e-08))}
+ � � � number=1
***MATCHING****
.PARAM vtor_alpha = {7.2e-09}
.PARAM vtor_beta �= {0}
.PARAM vtor_fudge �= {1}
.PARAM betsq_alpha = {1.85e-08}
.PARAM betsq_beta �= {0}
.PARAM betsq_fudge �= {1}
.PARAM vtor_sig = {((vtor_alpha/sqrt(W*L*number))+vtor_beta)*vtor_fudge/sqrt(2.0)}
.PARAM vtor_dev = 0.0 DEV/gauss = {vtor_sig*mismatch}
.PARAM betsq_sig = {((betsq_alpha/sqrt(W*L*number))+betsq_beta)*betsq_fudge/sqrt(2.0)}
.PARAM betsq_dev = 0.0 DEV/gauss = {betsq_sig*mismatch}

First I tried spice parser (option +csfe). It didn't like function trunc . The Spice homologue of Eldo trunc is int. When I replace trunc by int, spice parcer gives error.

Then I tried Spectre parser. I replaced .PARAM by parameters and trunc by floor. This was Ok. Problem rised with vtor_dev and betsq_dev parameters. For Spectre such syntax is uncomprehesible.

In which directio should I follow (adaptation to Spectre or Spice) and how could I circumvent problems mentionned above.

Quote:

.so is a "shared object" -- similar to a DLL in Windows. �Eg, the libphilips_sh.so contains the Mextram and PSP transistor models.

If I properly undestand you, the contents of this file is compiled models. So, it should be the way to use them? How?

Regards.

Pavel.

Back to top

IP Logged

imd1

Junior Member

Offline

Posts: 27

Re: using Eldo models in Spectre?
Reply #7 - May 9^th, 2007, 1:45am

Your kit uses an intermediate step between the actual transistor instantiation and the model parameter call.
So your problem is this intermediate step (the .SUBCKT call). I'd expect Spectre's SPICE reader to undertand Int()... Do you have a HSPICE compatible option for the spectre reader?

DEV/gauss in the .param is an ELDO idiom to specify the pdf of that .param for Monte-Carlo simulation. If you don't care much for it at this step you could just remove it. Spectre has probably a totally different way to define a probability distribution for a simulation parameter, which in this case is not a model parameter, but simply a subcircuit parameter (local to the subcircuit...).

I'd skip this and just get the normal simulation to run, and study later how the ELDO way differs from the Spectre way.

The .so seem to be external models using the CMI (Compiled Models Interface). It's curious that they are being loaded at all, since you do not need those models in your circuit... Apparently Spectre has all its MOS models as CMI .so files.

I don't know if the CMI interface for Spectre is publicly documented, if that's your question. Do you want to write/compile new models for it?

Back to top

IP Logged

Pavel

Senior Member

Offline

Posts: 174
Lausanne/Switzerland

Re: using Eldo models in Spectre?
Reply #8 - May 9^th, 2007, 4:22am

Hello imd1. Thanks for response. Some question concerning your advices.

Quote:

Your kit uses an intermediate step between the actual transistor instantiation and the model parameter call.
So your problem is this intermediate step (the .SUBCKT call). I'd expect Spectre's SPICE reader to undertand Int()... Do you have a HSPICE compatible option for the spectre reader?

What does "intermediate step" mean? When using Spectre parser I, of course, suppress the point.
So where is the problem? For Spice compatibility I use +csfe flag. With this flag Spice parser is used �(as I understood). But in this case another problem rises - trunc function. When I try replace trunc by int, parser gives an error.

Quote:

The .so seem to be external models using the CMI (Compiled Models Interface). It's curious that they are being loaded at all, since you do not need those models in your circuit... Apparently Spectre has all its MOS models as CMI .so files.

I didn't really understand what is the contents of this file. It isn't loaded. I've just founded it it Design Kit.
My question is : can it be used in some way or not?

Regards.

Pavel.

Back to top

IP Logged

Geoffrey_Coram

Senior Fellow

Offline

Posts: 1999
Massachusetts, USA

Re: using Eldo models in Spectre?
Reply #9 - May 9^th, 2007, 4:43am

imd1 wrote on May 9^th, 2007, 1:45am:

Your kit uses an intermediate step between the actual transistor instantiation and the model parameter call.

A simpler structure would be something like
M1 d g s b nch l=0.18u w=10u
.MODEL nch nmos level=60
But you have an instance of "ENULLMM9JU" that resolves to a .SUBCKT rather than a .MODEL. Indeed, I would try to figure out how to get the "nominal" simulation to run and then worry about mismatch later, as imd1 suggests.

Quote:

The .so seem to be external models using the CMI (Compiled Models Interface). It's curious that they are being loaded at all, since you do not need those models in your circuit... Apparently Spectre has all its MOS models as CMI .so files.

I don't think BSIM3/4 are .so files.

Quote:

I don't know if the CMI interface for Spectre is publicly documented, if that's your question. Do you want to write/compile new models for it?

It's not; last time I asked, Cadence wanted an NDA. I think you also need a license key.

Back to top

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

IP Logged

Geoffrey_Coram

Senior Fellow

Offline

Posts: 1999
Massachusetts, USA

Re: using Eldo models in Spectre?
Reply #10 - May 9^th, 2007, 4:48am

Pavel wrote on May 9^th, 2007, 4:22am:

I didn't really understand what is the contents of this file. It isn't loaded. I've just founded it it Design Kit.
My question is : can it be used in some way or not?

It will automatically be loaded if it is needed. If you have
.model nch nmos level=14 vth0=0.7 ...
then this is a BSIM4 model, and the model equations that go with these parameters are built into Spectre.

If you have
model nch psp1020 tox=1.5n ...
then Spectre will load the philips .so file for the equations for the PSP model. But the equations are useless without the appropriate parameters.

If you do a "spectre -help", near the end there is a list of components, with * for those that are loaded from shared objects (.so).

Back to top

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

IP Logged

Pavel

Senior Member

Offline

Posts: 174
Lausanne/Switzerland

Re: using Eldo models in Spectre?
Reply #11 - May 14^th, 2007, 3:41am

Quote:

DEV/gauss in the .param is an ELDO idiom to specify the pdf of that .param for Monte-Carlo simulation. If you don't care much for it at this step you could just remove it. Spectre has probably a totally different way to define a probability distribution for a simulation parameter, which in this case is not a model parameter, but simply a subcircuit parameter (local to the subcircuit...).

Quote:

A simpler structure would be something like
M1 d g s b nch l=0.18u w=10u
.MODEL nch nmos level=60
But you have an instance of "ENULLMM9JU" that resolves to a .SUBCKT rather than a .MODEL. Indeed, I would try to figure out how to get the "nominal" simulation to run and then worry about mismatch later, as imd1 suggests.

I tried as you suggested - suppresed Monte-Carlo statements. I also changed parameter names to lowercase to be them compatible with Spectre bsim4 parameters. Then I tried to generate netlist for small test schema (please, see on the picture).

Results
- parser passes without errors
- nmos isn't present in netlist
- in Spectre log window I see following information:

Notice from spectre during topology check.
Only one connection to the following 2 nodes:
drain
gate

Circuit inventory:
nodes 3
equations 5
resistor 1
vsource 2

Nmos isn't recognized, but parser passes without errors. Why?

Regards.

Pavel.

Back to top

test_bsim4_eldo.jpg

IP Logged

Pavel

Senior Member

Offline

Posts: 174
Lausanne/Switzerland

Re: using Eldo models in Spectre?
Reply #12 - May 14^th, 2007, 5:22am

Previous error is corrected. I included eldo in Switch & Stop View Lists in ADE/Setup/Environment Options/.
nmos appears in netlist.

Now problem is with model. Here is error message from spectre log window:
Error found by spectre during circuit read-in.
� �"........./test_lib.lib" 126: Bad `subckt ... ENLLMM9JU' statement.

Where 126 is the last line in the file test_lib.lib.
it sounds like this:
ends ENLLMM9JU
what is conform with Spectre syntax.

Where is the problem?

Regards.

Pavel.

Back to top

IP Logged

Geoffrey_Coram Senior Fellow Offline Posts: 1999 Massachusetts, USA	Re: using Eldo models in Spectre? Reply #13 - May 14^th, 2007, 6:38am In spice format, it's .subckt and .ends; in spectre, there's no leading "." I can't tell from your post which one you are intending to use. I don't remember whether either allows/requires/forbids having the subckt name on the "ends" line.
Back to top	If at first you do succeed, STOP, raise your standards, and stop wasting your time. IP Logged

Pavel Senior Member Offline Posts: 174 Lausanne/Switzerland	Re: using Eldo models in Spectre? Reply #14 - May 14^th, 2007, 6:51am Geoffrey, I don't use leading "." According to manual subckt name after ends is allowed. In any way I tried 2 options - with and without. Regards. Pavel.
Back to top	IP Logged