Stats

  • Locked Locked
  • Replies 3
  • Subscribers 64
  • Views 18754
  • 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

Convergence Issue

Charanraj Mohan

Hey I am using Cadence IC 6.1.6 & UMC 130nm technology

I have a big schematic and am running simulation in transient of 100us simulation time. I face some difficulties with convergence issues for which I tried the following-

1. With 'trap' the simulation becomes slower at 41%. Before 41% the step was in nano second and micro second.At 41% it became to Armstrong and femto seconds and became dead slow. In fact it did not cross 41 % simulation time. I lost my patience after i ran for several minutes. But I could see the expected output until 41% simulation time.

2. When I tried 'Euler', the same happened at 10.7% of simulation time i.e. in the beginning itself.

3. When I tried 'traponly' i get same results as in 1. But I get trapezoidal ringing at 4 nodes along with the expected output until 41% simulation time as observed in 1.

4. When I tried 'gear2', I get convergence problem at 7.28% of simulation time.

5. For 'gear2only' the convergence problem occurs at 6.5% of simulation time.

6. For 'trapgear2', it occurs at 8.49 % simulation time.

In 'trap' method there is no convergence issue until 40 us. After this only I get problems.

I have two questions-

a. How should I handle these non convergences ?

b. Is there any accelerator option in Cadence IC 6.1.6 simulation as in MATLAB ?

thanks in advance

  • First of all, it's the MMSIM version that matters here, not the IC version. Given the level of detail you've provided, I would suggest:

    1. Make sure you're using MMSIM14.1 or MMSIM15.1 (or at a pinch, MMSIM13.1 Update release or later - so you'd have 13.1.1 in the simulator version)
    2. In the Setup->Environment in ADE add +diagnose onto the userCmdLineOption field. This will print detailed diagnostics as to what might be causing the timestep issues.
    3. Yes, under Setup->High Performance Simulation you can turn on "APS" which is the Accelerated Parallel Simulator option for spectre. That won't necessarily solve your convergence problems though (it might, but it most likely is something you need to diagnose carefully). Usually it's a circuit (or sometimes a model) problem.

    Regards,

    Andrew.

  • Thanks Andrew.

    :-)

    I sorted it. I enabled 'allglobal' in refrel of accuracy parameter option in simulation. Then when I ran the simulation, there was no convergence problem. Earlier it was 'sigglobal' by default.

    It seems that each kit has its own default convergence settings & it simulates by it unless we change the options.

  • Typically the value of relref is dependent upon what errpreset you have set, so it may not be a PDK setting.

    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.