Stats

  • Locked Locked
  • Replies 24
  • Subscribers 126
  • Views 29052
  • Members are here 0
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Sweeping Vth vs L

Arjun RP

Hi all,

I am Arjun, Graduate student pursuing IC Design. I am trying to sweep the Vth of transistor with respect to its length. I saved a file with .scs extension and with the content save M0:all. I selected DC analysis and in the sweep i selected component parameter and transistor M0 where i selected its length "l". I also included the .scs file into model library. But when i run the simulation i am getting a error as given below. 

ERROR (SFE-430) : 'dc' : Sweeping the parameters of a subcircuit instance ('M0') is currently not supported. Please use the spectre sweep instead.

Spectre terminated prematurely due to fatal error.

 What should i do to overcome this error ? Please help me 

  •  Hi Arjun,

     try to use for the length of the device a variable for example 'n_length' (in the 'Edit Object Properties' form). Then choose in the DC analysis form instead of component parameter your design variable (n_length) as sweep variable.

     Regards

  • Thanks for replying. How can I sweep Vth wrt L if I add a variable name for length in edit properties of a transistor ? Can you please explain me the steps

  •  

     Hi,

     in ADEL clikc on Variables -> Copy From Cellview to load the length variable. I have attached a picture for the suggested DC analysis setup. Instead of typing the name of the variablein the 'Variable Name' field you can also click on 'Select Design Variable' and select your sweep variable.

     Regards

  • I did the steps mentioned by you. I can plot Id vs L. But i cant plot Vth vs L. After simulation if i go to results browser i couldnt see the Vth of the transistor in dc-dc tab. Only in dcOpInfo-info i can see Vth. But that gives only the value of Vth. I doesnt plot Vth vs L as it is operating point simulation. How should i plot Vth vs L from the results browser ?
  • I am also getting the following warnings if i use save M0:all and save M0:vth commands in .scs file 

  • The warnings are consistent with what I guessed might be the problem - I suspect that the model is a subckt and so saving M0:all is not correct - you need to save M0.instNameOfTransistor:all (where instNameOfTransistor is the name of the instance within the subckt model). You'll need to look in the model files to find out the name of the instance.

    Alternatively, use:

     save *:all devtype=bsim4

    which will save everything for all bsim4 instances - so that should do it. Might be simpler than trying to figure out the instance name...

    Regards,

    Andrew.

  • Hi ,

    I used this command save *:all devtype=bsim4 in my file. Now there is no warning but still i couldnt find the vth in dc-dc of the results browser 

  • Which simulator version are you using? I just ran this netlist:

    // simple example of a dc sweep of length
    parameters length=1u
    subckt nch (d g s b)
     parameters w=1u l=1u
     M1 (d g s b) nch w=w l=l
     model nch bsim4 type=n
    ends nch

    M0 (d g 0 0) nch w=1u l=length
    VD (d 0) vsource dc=1
    VG (g 0) vsource dc=1

    save *:all devtype=bsim4
    dc dc param=length start=0.5u stop=10u step=0.5u

    and got the results below in the results browser.

    Regards,

    Andrew.

  • I am using Virtuoso 6.1.4 (Virtuoso ADE IC6.1.4.500.5) - as seen from Help-->About ADE . I am a student so am not much experienced with running the netlist you have provided. If you can guide me step by step it will be very helpful for me. 

  • It's the simulator I'm more interested in (so look at the top of the spectre output file to see the subversion).

    I just tried with the same IC version you're using and that worked - see the picture (this was simulated with an MMSIM11.1 simulator version just arbitrarily).

    To run it, put the contents in a file called "vtsweep.scs" and then run "spectre vtsweep.scs". I ran "viva" and then opened vtsweep.raw and plotted the results.

    Regards,

    Andrew.

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.