Home > Community > Forums > Mixed-Signal Design > Model parameters

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: *

 Model parameters 

Last post Wed, Aug 6 2014 1:39 AM by Arjun RP. 13 replies.
Started by ag2888 28 Mar 2013 01:24 AM. Topic has 13 replies and 5997 views
Page 1 of 1 (14 items)
Sort Posts:
  • Thu, Mar 28 2013 1:24 AM

    • ag2888
    • Top 500 Contributor
    • Joined on Thu, Mar 28 2013
    • Posts 18
    • Points 335
    Model parameters Reply

    Hi,

    I am trying to get an idea as to what a device model parameter represents.
    Can anyone please suggest where i can get the list for it.
    I am specifically looking for the parameters like mobility, Cox, subthreshold factor, TC of threshold voltage, Vth0 of the device etc.

    Also i am trying to plot the threshold voltage of a device as per my DC sweep parameter. Can anyone please tell me how should i do that?

     

     

    • Post Points: 20
  • Fri, Mar 29 2013 8:06 AM

    Re: Model parameters Reply

    Did you consider reading the documentation? There's a whole manual on the device model equations, plus documentation on the parameters available for each mode. Run "cdnshelp" from <MMSIMinstDir>/tools/bin to get to the documentation.

    If you want to plot the threshold voltage, the best thing to do is to create an include file, called (say) save.scs with the contents:

    save M1:vth

    and then reference this file from Setup->Model Libraries or Setup->Simulation Files. Then you can see this parameter from the Results browser after your dc sweep. Of course, change M1 to be whatever the device name is in your case.

    Regards,

    Andrew.

    • Post Points: 20
  • Tue, Aug 13 2013 11:17 AM

    • Alex Liao
    • Top 150 Contributor
    • Joined on Wed, May 22 2013
    • Posts 47
    • Points 775
    Re: Model parameters Reply

    Hi Andrew,

     

    I went through this thread and am interested in plot vth through DC sweep. But I received this warning´╝Ü

       WARNING (SPECTRE-8282): `M1a' is not a device or subcircuit instance name.

        WARNING (SPECTRE-8287): Ignoring invalid item `M1a:vth' in save statement.

        WARNING (SPECTRE-8282): `M6' is not a device or subcircuit instance name.

        WARNING (SPECTRE-8287): Ignoring invalid item `M6:vth' in save statement.

    I am sure the name is correct and is copied from schematic instance name field.  

     Do you know how to fix it?

     

    Thanks,

     Alex

    • Post Points: 20
  • Tue, Aug 27 2013 2:13 PM

    Re: Model parameters Reply

    Presumably the name is not correct, or you've not given the correct hierarchical path to the instance. Look at the netlist itself - that's the best bet.

    Regards,

    Andrew.

    • Post Points: 20
  • Tue, Aug 27 2013 2:44 PM

    • Alex Liao
    • Top 150 Contributor
    • Joined on Wed, May 22 2013
    • Posts 47
    • Points 775
    Re: Model parameters Reply

    Hi Andrew,

    You can refer my snap cut. The naming is correct. I do not know how to check that hierarchical path. But the netlist is enough I think. 

     Regards,

    Alex 

    • Post Points: 20
  • Tue, Aug 27 2013 2:52 PM

    Re: Model parameters Reply

    Alex,

    The transistors you're trying to save the vth for are inside the _sub0 subckt, and you didn't tell it the hierarchical path to them. Since there is only one instance of that subckt, ie instance I0, you'd need:

    save I0.M1a:vth

    (assuming that the model pch is not a subckt itself).

    Regards,

    Andrew 

    • Post Points: 20
  • Wed, Aug 28 2013 1:39 PM

    • Alex Liao
    • Top 150 Contributor
    • Joined on Wed, May 22 2013
    • Posts 47
    • Points 775
    Re: Model parameters Reply

    Hi Andrew,

     In my case I have seen that subckt _sub0.  But wher is the instance info? As you exampled, the instance I0, what is the only instance name in my design from previous snapshoot?

     Thanks,

    Alex 

    • Post Points: 20
  • Thu, Aug 29 2013 1:21 AM

    Re: Model parameters Reply

    Alex,

    All I did was read your netlist in your post. It's not difficult!

     


    • Post Points: 20
  • Thu, Aug 29 2013 2:10 PM

    • Alex Liao
    • Top 150 Contributor
    • Joined on Wed, May 22 2013
    • Posts 47
    • Points 775
    Re: Model parameters Reply

    Andrew,

    I have no warning now. I assume that I have saved vth of M6 by including "save I0.M6.vth". But this thread mentioned plot this variance by DC sweeping. How can I plot it with the help of result browser. You can point it out direct in this figure .

    Thanks,

    Alex 

    • Post Points: 20
  • Fri, Aug 30 2013 12:27 AM

    Re: Model parameters Reply

    Alex,

    Firstly it would be "save I0.M6:vth" (note the colon) - check the spectre output as it will tell you if you have got it wrong.

    Secondly, you're looking at the dcOp output there, not the dc sweep output. That's the (initial) DC operating point. You'd need to look in the "dc-dc" output in the results browser, and then you should be able to plot a waveform of I0.M6:vth versus the swept parameter.

    Kind Regards,

    Andrew.

    • Post Points: 20
  • Fri, Aug 30 2013 9:42 AM

    • Alex Liao
    • Top 150 Contributor
    • Joined on Wed, May 22 2013
    • Posts 47
    • Points 775
    Re: Model parameters Reply

    Hi Andrew,

     Thank you so much. Now I have my desired plot.

     

    Regards,

    Alex. 

    • Post Points: 20
  • Wed, Aug 6 2014 1:16 AM

    • Arjun RP
    • Not Ranked
    • Joined on Tue, Aug 5 2014
    • Singapore, 00-SG
    • Posts 16
    • Points 245
    Re: Model parameters Reply

    Hi,

     I am trying to plot Vth vs L like the same manner as described in your post. I gave a variable name in length field of transistor and chose dc analysis. In that i selected design variable as sweep variable and added the variable name. But when im running the simulation i am getting the following error.  Even if i give save M0:vth , im getting error and in the results browser (dc-dc) there is no Vth of the tansistor. Please help me in this regard. 


    • Post Points: 20
  • Wed, Aug 6 2014 1:29 AM

    Re: Model parameters Reply

    Please read the forum guidelines - these tell you not to double post (especially when you already have your own thread on this subject). I answered your other post here.

    • Post Points: 20
  • Wed, Aug 6 2014 1:39 AM

    • Arjun RP
    • Not Ranked
    • Joined on Tue, Aug 5 2014
    • Singapore, 00-SG
    • Posts 16
    • Points 245
    Re: Model parameters Reply
    Oh sorry i didnt see the guidelines. I saw this post in the meanwhile that was having similar error as mine. So posted my error in this post. Sorry for the double post . 
    • Post Points: 5
Page 1 of 1 (14 items)
Sort Posts:
Started by ag2888 at 28 Mar 2013 01:24 AM. Topic has 13 replies.