Stats

  • Locked Locked
  • Replies 3
  • Subscribers 126
  • Views 7084
  • 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 copy designs to different machines?

Doronzzz

I am trying to copy the OTA I designed from my local workstation to a remote server. I just opened a new project on the server and manually copied the sizing of each transistor. The strange thing is that the two designs has different DC operating points... 

The PDKs on the two machines are both from smic 180nm technology, but I don't know if they are exactly the same. The transistor models I used have the same name "n18_ckt", so I assumed they are the same model. I will check the model parameters after DC simulations next, to see if the models are the same indeed.

So my questions are: 

1) What might possibly cause this problem? 

I've checked the process corner used on the two machines, they are both called xxx_tt. The simulation temp are the same (25 degrees). What else could affect the outcome of a simulation?

2) What is the recommended way to copy designs across different machines?

Is there something like Git on Cadence?

Thanks in advance.

Parents

  • Dear Doronzzz,

    Doronzzz said:
    ) What might possibly cause this problem? 

    Wow! A lot of questions and no firm answers from me based on the information you provided, but I can add a few suggestions. I am sure other experts who monitor this Forum may have other and, perhaps better, suggestions.

    1. If the DC operating points of two presumably identical schematic based netlists are different, there are numerous causes.

    a. First, compare the input.scs files of both simulations - i.e, compare the input.scs file generated in your local workstation environment and the input.scs file generated on the remote server. The "input.scs" file is contained in the netlist directory.  Based on your intent, the two should be identical. If not, study your two schematics and determine if there is a difference responsible for the difference.

    b. Compare the runSimulation files (also in the netlist directory) for both your local workstation and remote server. This file contains the full set of spectre options. Verify that the same options are used for both simulations.

    c. Compare the two spectre.out log files for the two simulations. Specifically, verify the versions of the Cadence tools used is identical and that they both are using the same simulator (i.e, spectre, spectre +aps, or spectre ++aps). You should also be able to tell the version of the model files used and hence verify that the model versions are identical for the two simulations.

    As an example, in a sample spectre.out file I happen to have, the second line states the Cadence tool version as:

    Spectre (R) Circuit Simulator
    Version 20.1.0.382.isr12 64bit -- 5 Nov 2021

    Further down in the file is the simulation line, for example:

    Command line:
    /tools/MMSIM/20.10.382.ISR12/Linux/tools/bin/spectre -64 input.scs \
    +escchars +log ../psf/spectre.out -format psfxl -raw ../psf \
    +aps=conservative +mt=lsf +lqtimeout 0 -maxw 5 -maxn 5 -env ade \
    +disk_check=100e9 -ahdllibdir \

    There should also be some indication of the model file(s) used which often contains the model version number in its path.

    2. You might also try copying the input.scs file and the runSimulation files from one environment to the other and manually run the command line to verify the copied input.scs and runSimulation files produce the same simulation results.

    Doronzzz said:

    2) What is the recommended way to copy designs across different machines?

    Is there something like Git on Cadence?

    Using the Library Manager is a far more efficient means of copying one schematic from one library to a different library. While I do not believe Cadence offers a tool for version control, there are third parties that provide version control that work flawlessly with Cadence's Library Manager. 

    Shawn

  • in reply to ShawnLogan

    Hello Shawn,

    Thanks so much for your suggestions!

    I compared the model versions and found this to be the cause of the problem. The two PDK versions do have some differences, I didn't expect them to make a huge difference, even though they belong to the same technology node. 

    I'll check other things you've mentioned as well. I believe they will be of great help in understanding how simulations work.

    Thanks!

    Doronzzz

Reply
  • in reply to ShawnLogan

    Hello Shawn,

    Thanks so much for your suggestions!

    I compared the model versions and found this to be the cause of the problem. The two PDK versions do have some differences, I didn't expect them to make a huge difference, even though they belong to the same technology node. 

    I'll check other things you've mentioned as well. I believe they will be of great help in understanding how simulations work.

    Thanks!

    Doronzzz

Children

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.