Stats

  • Locked Locked
  • Replies 3
  • Subscribers 125
  • Views 14010
  • 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

ADEXL different accuracy setting for sub-blocks

TaoC

Hi,

I'm doing a large post-layout circuit transient simulation. I only need high accuracy on part of the entire circuit. Using "conservative" will be applied to the entire netlist and it will slow down the simulation. Is there a way to only specify some transistors to be "conservative", while the rest to be "liberal"?

Thanks,

-Tao

  • Dear TaoC,

    TaoC said:
    I only need high accuracy on part of the entire circuit. Using "conservative" will be applied to the entire netlist and it will slow down the simulation. Is there a way to only specify some transistors to be "conservative", while the rest to be "liberal"?

    Did you happen to review the Spectre Manual at URL:

    support.cadence.com/.../ArticleAttachmentPortal

    Under the heading "Sweeping Parameters During Transient Analysis", which I copied and included below,  the manual notes that the value of errpreset can be changed locally at the subcircuit level using the keyword "sub=<subcircuit_name>" with the "param_name" set to param="errpreset".

    This allows, for example, an errpreset of "conservative" for a critical analog circuit while a less time intensive value of errpreset may be used for a digital, low speed, portion of the netlist.

    I hope I understood your question!

    Shawn

    Sweeping Parameters During Transient Analysis

    You can modify temperature, tolerance, and design parameter settings at device, subcircuit, or model level during a transient analysis. The syntax is:

    Name tran param=param_name, { param_vec=[ t1 val1 t2 val2...] | param_file=file }, [ dev=d1 | mod=m1 | sub=s1 ], param_step=time

    where

    Name

    Name of the transient analysis.

    param=param_name

    Dynamic parameter name. The parameter name can be a design parameter, errpreset, method, relref, maxstep, isnoisy, lteratio, reltol, residualtol, vabstol, iabstol, temp, and tnom.

    param_vec=[ t1 val1 t2 val2...]

    Time points and values of the parameter.

    param_file=file

    File name if the param_vec is defined in a separate file.

    dev=d1 | mod=m1 | sub=s1

    Defines local scope for design parameters. Can be a device model instance (dev), device model name (mod), or subcircuit instance name (sub). Does not apply to temp, reltol, residualtol, vabstol, iabstol, or isnoisy.

    param_step=time

    Specifies whether the time_value pair given by the param_vec parameter is to be updated in one step, or as a series of steps. See Examples 1 and 2 below. Default value: 0

    faultreadic

    Specifies the file that contains the initial condition (ic) information related to fault sensitivity analysis.
  • in reply to ShawnLogan

    Thank you Shawn! This is exactly what I need. In the ADE gui, I also found this dynamic parameter option. But it seems that I can only select the param vector. Is it possible to add subcircuit in the ADE GUI window? 

  • in reply to TaoC

    Dear TaoC,

    TaoC said:
    I also found this dynamic parameter option. But it seems that I can only select the param vector. Is it possible to add subcircuit in the ADE GUI window? 

    I am happy to read I understood your question!

    I think you might use the additional parameter entry box in the Misc tab of the transient analysis panel I've highlighted in Figure 1 to include the syntax shown in the  reference manual. To verify this, create a netlist and verify that the transient analysis command contains both the errpreset value you desired and the "sub=" you entered in the additional parameter box. I dud not try this, so that is why I am recommending you verify it provides the proper syntax in the input.scs file.

    Shawn

    Figure 1

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.