The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> Hspice model file in Spectre
https://designers-guide.org/forum/YaBB.pl?num=1157105457

Message started by xwcwc1234 on Sep 1^st, 2006, 3:10am

Title: Hspice model file in Spectre
Post by xwcwc1234 on Sep 1^st, 2006, 3:10am

Hi,
I am new to spectre . Now I want to simulate my circuit with Spectre use Hspice model file that provide by foundry . Could anyone of you help me in this regard of by providing spectre simulation statements required for this requirement ?

Title: Re: Hspice model file in Spectre
Post by byang on Sep 1^st, 2006, 8:35pm

Hi, xwcwc1234,

In Spectre, you can use simulator lang=spice to include HSPICE model file. I am wondering why you want to use Spectre simulator but have HSPICE model file. Doesn't the foundry provide Spectre model file too?

Baolin

Title: Re: Hspice model file in Spectre
Post by xwcwc1234 on Sep 6^th, 2006, 2:01am

Hi byang,
Thanks for your reply. Indeed , the foundry did not supply Spectre model file , only hspice model file available.
When I use spp to convert Hspice model file to Spectre's , some warning messages show as below :
`ng.1': `nlev' is not a valid parameter for `bsim3v3' models.
`ng.1': `acm' is not a valid parameter for `bsim3v3' models.
`ng.1': `calcacm' is not a valid parameter for `bsim3v3' models.
`ng.1': `sfvtflag' is not a valid parameter for `bsim3v3' models.
`ng.1': `vfbflag' is not a valid parameter for `bsim3v3' models.
That means some Bsim3v3 parameters of Hspice level 49 are not recognized by Spectre . I use Spectre 4.4.6 , is that too old ?

Title: Re: Hspice model file in Spectre
Post by Geoffrey_Coram on Sep 6^th, 2006, 6:53am

xwcwc1234 wrote on Sep 6^th, 2006, 2:01am:

I use Spectre 4.4.6 , is that too old ?

That's verging on ancient ...

Title: Re: Hspice model file in Spectre
Post by Andrew Beckett on Sep 20^th, 2006, 3:05am

Recent versions of spectre (MMSIM60 onwards, although it could be enabled in IC5141's spectre by using the +csfe command line switch) have a new front end which natively reads SPICE netlists and models as well as spectre's own netlist language. Whilst in older versions spectre did have some limited SPICE language support, for the most part it was done using a pre-processor (called "spp"). You could always use spp to convert the models, but the best approach is really to use a more recent simulator (which doesn't require spp). There have been a lot of advances since IC446, and there is no benefit in using such an old version of the simulator!

Andrew.

Title: Re: Hspice model file in Spectre
Post by simon2 on Sep 23^rd, 2007, 4:16am

Hi xwcwc1234,
I can appreciate where perhaps one may be in a situation where you are stuck with the simulator of someone else's choice (which may be an older version of spectre-cadence) or perhaps have to support someone who does not use cadence tools (for example an external design house or foundry provider) which means that you maynot be able to go to the latest version of the Cadence tools.

The solution I use is to maintain a set of test-benches that re-run the process "playbacks" (published in the Foundry documentation) for each device. These test-benches use the same "test" circuit, but call different model files for (say) nmos or pmos or npn or a diode and will become over time a superset of all the processes you use (mine are now about 8 years old and cover some 20 processes). I maintain these for each tool-set/simulator we support, adding new tools and processes as they become available allowing us to verify model accuracy, parameter coverage, model robustness and so on.

Having built such a knowledge base, you will then be able to look at parameters such as those above and decide which matter to the application you are designing for - some such as those listed above may not, so comment them out in model file (remember to keep a backup of the originals just in case you completely break the model).

I would strongly recommend that you read a book such as "MOSFET Modeling and BSIM3 User's Guide" by Cheng and Hu, to get an idea of what these parameters do and if they matter to you. In time you will find that you can write sub-circuits that add these features if necessary, or even produce you own bespoke model files that emulate the behavior the "extra" parameters pertain to, even though the simulator does not directly model those parameters.

You will find after a while that you are only limited your ability rather than the tools - they just make the challenge interesting, the point being that you will have to start your design somewhere and the re-simulating the foundry playbacks in your simulator make an excellent starting point.

Cheers,
SimonH.