Home > Community > Forums > Custom IC Design > Is there a way to print model parameter using Hspice-D version2012.03 after running a simulation?

Email

* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

 Is there a way to print model parameter using Hspice-D version2012.03 after running a simulation?  

Last post Sat, Aug 31 2013 9:02 AM by Andrew Beckett. 9 replies.
Started by Alex Liao 28 Aug 2013 03:37 PM. Topic has 9 replies and 917 views
Page 1 of 1 (10 items)
Sort Posts:
  • Wed, Aug 28 2013 3:37 PM

    • Alex Liao
    • Top 200 Contributor
    • Joined on Wed, May 22 2013
    • Posts 41
    • Points 655
    Is there a way to print model parameter using Hspice-D version2012.03 after running a simulation? Reply

    Based on my knowledge, I use Spectre simulator and after simulation, through Results=> Print Tab, I could print model parameter. While in Hspice is there a similar trick to do this? Any reply is appreciated.

    Thanks,

    Alex. 

    • Post Points: 20
  • Thu, Aug 29 2013 1:46 AM

    Re: Is there a way to print model parameter using Hspice-D version2012.03 after running a simulation? Reply

    Alex,

    I don't think you can do that (I don't know for sure because I don't have access to that HSPICE version - it's probably best to ask Synopsys since it is their simulator) - but HSPICE writes the model parameters into the simulator output log:

     ************************************************************************
     ***************************************************************************
     ***        model parameters  model name:   0:pch      model type:pmos   ***
     ***************************************************************************

       *** general parameters ***
        deriv=   0.          

       ***  level 49  model parameters  ***

          hspver=    2006.03               level=         49        
         version=        3.3            paramchk=          0        
          apwarn=          1                lite=          0        
          vgslim=          0             binUnit=          1        
          capMod=          3               xpart=          1        
          mobMod=          1              nqsMod=          0        
        acnqsMod=          0              stiMod=          0        
             elm=          5            sfvtflag=          0        
             tox=    1.2e-08 meter            xj=    1.5e-07 meter  
     

    Kind Regards,

    Andrew.

    • Post Points: 20
  • Thu, Aug 29 2013 2:36 PM

    • Alex Liao
    • Top 200 Contributor
    • Joined on Wed, May 22 2013
    • Posts 41
    • Points 655
    Re: Is there a way to print model parameter using Hspice-D version2012.03 after running a simulation? Reply

    Andrew,

    This may partially relates to this topic, but I just noticed that in Spectre Manual (Virtuoso Simulator Components and

    Device Models Reference, V12.11 May 2013),  there are two instance parameters.

    One is:

    19 mulu0=1 mobility multiplier. in BSIM3v3 Level-11 Model(bsim3v3) or  65 mulmu0=1.0 Mobility multiplier, alias of mulu0 in BSIM4 Level-14 Model (bsim4).

     Another one is:

    17 delvto=0 V shift in zer0-bias threshold voltage vth0 in Bsim3v3. or  in Bsim4.5 "A new instance parameter DELVTO that may be used to represent threshold voltage variation" And even the equation for delvto is given .

    However, these two parameters are only found in manual, not in model cards, or pint model parameters(psf) after simulation. Do they really exist and if so how to retrirve them? In Hspice 2010 vertion manual, these two are given in more detail. But I check hspice.out, still no appearance as well as  in model card. It looks both hspic and spectre documented them but I put a question mark on whether any simulator uses them.

    Regards,

    Alex.

     

    • Post Points: 20
  • Fri, Aug 30 2013 12:37 AM

    Re: Is there a way to print model parameter using Hspice-D version2012.03 after running a simulation? Reply

    It's an instance parameter - so why would they appear in the model cards or in the printed model parameters? There is a difference between an instance parameter and a model parameter - model parametes are used in model cards, whereas instance parameters are used on the instance of the transistor (like w,l,ad,as, etc).

    With spectre, these would appear in the "instance" info database in the psf (use the results browser to access this).

    So why do you put a question mark on whether the simulator uses them?

    Regards,

    Andrew.

    • Post Points: 20
  • Fri, Aug 30 2013 10:48 AM

    • Alex Liao
    • Top 200 Contributor
    • Joined on Wed, May 22 2013
    • Posts 41
    • Points 655
    Re: Is there a way to print model parameter using Hspice-D version2012.03 after running a simulation? Reply

    Andrew,

    Fine, now I know those instance parameters are specified by users like w/l, or generated after simulation like mulu0.  In my snapshoot, , it seems those delvt0(V) = nan, mulu0 = nan, what does this mean? There should be certain validated values assigned for them. Also I checked the stimod field which is highlighted. It is stimod = 2147483647. I think this selector can only be 0/1/2.

     

    Regards,

    ALEX 

    • Post Points: 20
  • Fri, Aug 30 2013 2:05 PM

    Re: Is there a way to print model parameter using Hspice-D version2012.03 after running a simulation? Reply

    Alex,

    That means the parameters have not been set on the instance. nan (which stands for "Not A Number" - see this explanation) is being used for any floating point parameters, as it is effectively an invalid value - and just is used to mean that it wasn't set. For integer parameters such as stimod, it uses the largest possible positive 32 bit integer (the value corresponds to 2^31-1) to indicate the same thing - that it wasn't set on the instance.

    Regards,

    Andrew.

    • Post Points: 20
  • Fri, Aug 30 2013 2:40 PM

    • Alex Liao
    • Top 200 Contributor
    • Joined on Wed, May 22 2013
    • Posts 41
    • Points 655
    Re: Is there a way to print model parameter using Hspice-D version2012.03 after running a simulation? Reply

    Andrew,

     

    Is there a case that mulu0 and delvt0 has real value after simulation?

    If stimod is not set from element information, then why print model parameter can have stimod = 0. And in your case, you can change it by editing model card. Does this mean, not set then it is default value 0; set then copy seting from model card.

     

     Regards,

    Alex. 

    • Post Points: 20
  • Fri, Aug 30 2013 2:50 PM

    Re: Is there a way to print model parameter using Hspice-D version2012.03 after running a simulation? Reply

    Because (as I said before) setting the instance parameter doesn't change the model itself. The model parameter has a default value of 0 and that is what is displayed in the model parameters unless it has been set to something else in the model card. 

    I believe (and I'm guessing because I'm replying on a mobile device and have no means of testing this as it's late in my evening) that the instance's effective stimod is whatever is in the model card, or 0 if not set, but if set on the instance, that wins. 

    Regards,

    Andrew 

    • Post Points: 20
  • Fri, Aug 30 2013 3:55 PM

    • Alex Liao
    • Top 200 Contributor
    • Joined on Wed, May 22 2013
    • Posts 41
    • Points 655
    Re: Is there a way to print model parameter using Hspice-D version2012.03 after running a simulation? Reply

    [QUOTE=Andrew] Because (as I said before) setting the instance parameter doesn't change the model itself.

    .

    I now know the instance parameter is irrelated to model parameter. What I want to know is in what case the result browser can have instance paremeter mulmu0 and delvto not equal to nan, but a numerical value. If these two are forever set to nan and not uesd, why bother creating them?

    BTW, I wish you have a good weekend and only reply me if you feel comfortable. 

    Regards,

    Alex 

    • Post Points: 20
  • Sat, Aug 31 2013 9:02 AM

    Re: Is there a way to print model parameter using Hspice-D version2012.03 after running a simulation? Reply

    Alex,

    If they are specified on the instance line as in this following example (I added info analyses saving into "rawfile" so that I can see them in the results browser), then they'll show up (as in the picture attached):

    // example of setting stimod on a binned model
    parameters dxln=0.1u dxwn=0.1u

    model nch bsim4  {
         1: type=n
         + stimod = 2
         + lmin=9.999997e-006-dxln   lmax=2.00001e-05          wmin=1e-005-dxwn
         2: type=n
         + lmin=1u   lmax=2u          wmin=1u wmax=2u
         }

    M1 (1 2 0 0) nch w=12u l=11u delvto=0.1 mulmu0=1.1 stimod=1
    //M1 (1 2 0 0) nch w=1.2u l=1.1u

    modelParameter info what=models where=rawfile
    element info what=inst where=rawfile
    outputParameter info what=output where=rawfile

    Regards,

    Andrew.


    • Post Points: 5
Page 1 of 1 (10 items)
Sort Posts:
Started by Alex Liao at 28 Aug 2013 03:37 PM. Topic has 9 replies.