The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> Convert Hspice Level 49 Models into Spectre Models
https://designers-guide.org/forum/YaBB.pl?num=1224177312

Message started by essam on Oct 16^th, 2008, 10:15am

Title: Convert Hspice Level 49 Models into Spectre Models
Post by essam on Oct 16^th, 2008, 10:15am

Hi All,

I am working on a Switched Capacitor Filter Project. The Professor provided Hspice and TI Spice models only. I want to use Spectre Simulator. Spetre did not recognize the provided Level 49 Hspice models.

Is there a systematic way of conerting Hspice models into Spectre Models?

Thanks,
Essam

Title: Re: Convert Hspice Level 49 Models into Spectre Models
Post by Geoffrey_Coram on Oct 16^th, 2008, 11:53am

The latest version of Spectre should accept hspice models, you shouldn't even need a simulator lang=hspice statement if it's a .mod or .sp file.

What version of Spectre are you running?

level=49 is bsim3, so
.model nch nmos level=49 ...
should be the same as
model nch bsim3v3 type=n ...

Title: Re: Convert Hspice Level 49 Models into Spectre Models
Post by essam on Oct 16^th, 2008, 1:19pm

Hi,
Thanks for your reply.

I am not sure what version of spectre do we have, and honestly I do not know how to check that.

I attached the model file

Here is the rror message I am getting from Spectre.

Error found by spectre during circuit read-in.
"/net/core/export/home/ee/001/e/esa061000/Courses/Fall08/hspice_models/HModel5V1um.txt"
121: For .model `nch' of type `nmos', the value of level=49 is not
supported.
"/net/core/export/home/ee/001/e/esa061000/Courses/Fall08/hspice_models/HModel5V1um.txt"
237: For .model `pch' of type `pmos', the value of level=49 is not
supported.
"/net/core/export/home/ee/001/e/esa061000/Courses/Fall08/hspice_models/HModel5V1um.txt"
352: For .model `nat' of type `nmos', the value of level=49 is not
supported.

spectre terminated prematurely due to fatal error.

Thanks!

Essam

Title: Re: Convert Hspice Level 49 Models into Spectre Models
Post by Geoffrey_Coram on Oct 16^th, 2008, 1:52pm

essam wrote on Oct 16^th, 2008, 1:19pm:

I am not sure what version of spectre do we have, and honestly I do not know how to check that.

It should tell you at the top of the output; you can also do
spectre -W

I'm pretty sure you're using a rather old version.

Title: Re: Convert Hspice Level 49 Models into Spectre Models
Post by essam on Oct 16^th, 2008, 1:57pm

I found it: it is spectre er 5.0.33.070605

Thanks,
Essam

Title: Re: Convert Hspice Level 49 Models into Spectre Models
Post by Geoffrey_Coram on Oct 16^th, 2008, 2:06pm

Copy the file and change
.MODEL NCH NMOS
+ LEVEL = 49

to
model nch bsim3v3 type=n

(and type=p for PCH)

Title: Re: Convert Hspice Level 49 Models into Spectre Models
Post by essam on Oct 16^th, 2008, 2:13pm

I am getting exactly the same error message, after the changes you told

Title: Re: Convert Hspice Level 49 Models into Spectre Models
Post by Geoffrey_Coram on Oct 17^th, 2008, 7:20am

I meant for you to replace 2 lines with one; if you took out the LEVEL=49 line, then you shouldn't be getting the same error message.

Title: Re: Convert Hspice Level 49 Models into Spectre Models
Post by essam on Oct 17^th, 2008, 7:40am

That's what I have done but it did not work!!

Essam

Title: Re: Convert Hspice Level 49 Models into Spectre Models
Post by essam on Oct 17^th, 2008, 1:53pm

It seems that it reads and interprets the model parameters somehow and based on that say it is Level 49

Title: Re: Convert Hspice Level 49 Models into Spectre Models (SOLUTION FOUND)
Post by essam on Oct 18^th, 2008, 7:15am

HI,

I FOUND THE SOLUTION

Leave the model statement as is:

.Model nch nmos

But remove two lines:

+LEVEL = 49
+VERSION = 3.1

the simulator now runs but I need to check it versus hspice simulation to guarantee that the models are read without problems :)

Title: Re: Convert Hspice Level 49 Models into Spectre Models
Post by Andrew Beckett on Jan 2^nd, 2009, 3:27pm

Bit of a late response, but using spectre from a release in 2003 is probably not the wisest choice... there have been many, many improvements since then, including far better SPICE syntax and SPICE/HSPICE model compatibility. Using an MMSIM70 version of spectre would make far more sense.

Regards,

Andrew.