Stats

  • Locked Locked
  • Replies 6
  • Subscribers 127
  • Views 19576
  • 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

How to view the parameters inside VerilogA model after Spectre simulation?

Paulux

 Hello,

The resistor spectre model with VerilogA model are shown below. May I know how to view the parameter rl_va, rw_va & r_n inside VerilogA resistor model after Spectre simulation? How could I view these parameters using Result Browswer inside Virtuoso Analog Design Environment?

The reason I want to view because the default setting "scale=1e-6" is enabled and I need to check whether the values inside VerilogA will be or not be scaled by this "scale=1e-6".Also I want to double-check the values calculated inside VerilogA model.

Thank you for your kindness and help.

 

section res

ahdl_include "./res.va"

subckt rnpoly (1,2)

parameters rl=1 rw=1

+r_rsh0=65

+r_dw=2.05e-8

+r_dw=2.05e-8

rbody_r (1 2) res_va l=rl w=rw rsh0=r_rsh0 dw=r_dw dl=r_dl

ends rnpoly

 

Verilog A file (res.va) is shown below.

'include "discipline.h"

'include "constants.h"

module res_va(p, n);

inout p,n;

electrical p,n;

parameter real rsh0=65;

parameter real l=0;

parameter real w=0;

parameter real dl=0;

parameter real dw=0;

real rl_va, rw_va,r_n;

analog begin

rl_va=l-2*dl;

rw_va=w-2*dw;

r_n=r_l/r_w;

r=r_n*rsh0;

end

endmodule

  • You need to turn on the saveahdlvars=all option - which is on the Outputs->Save All form in ADE.

    Andrew.

  • Thank you very much for Andrew's useful reply.

    May I know where and how I can view the parameter value of rl_va, rw_va & r_n after turning on the saveahdlvars=all option?

    I cannot find the numerical values of (rl_va, rw_va & r_n) in any outputParameter-Info, modelParameter-info or designParamVals-info inside the Results Browser(Analog Design Environment->Tools)!

    Thank you for your kindness and help.

  • If you do a DC operating point simulation, you can see them in the dcOpInfo-info result database (even without turning on saveahdlvars). If you turn on saveahdlvars, you can also see them in the transient results (and plot them varying over time) - they'll also appear in the dcOp-dc database.

    They won't appear in the outputParameter-info (they're not device "output parameters"), modelParameter-info (they're not model parameters), or designParamVals-info (they're not design variables).

    Regards,

    Andrew.

  •  Hi,

      yes, just like andrew said.  i usually check it by resutls browser, you can see all of parameters values there.

    regards,

    zfeng

  • Hi Andrew,

    I am currently trying to use the latest BSIMSOI verilog-a code in Cadence (IC614). The problem is that,during simulation, the spectre seems to take the default value of the parameters written in the verilog-a code but not from the model card which I am providing in the ADE. Where do you think is the problem?

     Thanks 

  • Without seeing the model and the setup, it's very hard to answer this as I have no visibility of what you're doing. Maybe you can contact customer support.

    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.