Stats

  • Locked Locked
  • Replies 4
  • Subscribers 127
  • Views 3952
  • 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

Re-evaluating an "eval err" expression after simulation

RuihW

Hello,

I was running transient simulation on a large circuit in ADE Explorer,and it took 4 days to complete. However, it returned "eval errr" for the output expression. In my previous experience, it's likely due to an invalid expression so I'm working on fixing it. But I really don't want to spend another 4 days to run it, and even worse, that gives me another "eval err" at the end. Is it possible to update and re-evaluate an expression that returned "eval err" without re-running the simulation?

An additional question, the log of the transient simulation has these lines. Does that mean spectre had a convergence issue with homotopy = gmin? If I have to re-run the simulation, how can I let spectre to skip the first one and use homotopy = source directly? That'll likely save me 40% of the simulation time.

Trying `homotopy = gmin' for initial conditions.
Trying `homotopy = source' for initial conditions.
Notice from spectre during IC analysis, during transient analysis `tran'.
    GminDC = 1 pS is large enough to noticeably affect the DC solution.
        dV(I0.O0.OB0.OM825.I0.M13:int_d) = -119.442 mV
        Use the `gmin_check' option to eliminate or expand this report.
    Bad pivoting is found during DC analysis. Option dc_pivot_check=yes is recommended for possible improvement of convergence.

DC simulation time: CPU = 130.157 ks, elapsed = 130.186 ks.
Many thanks!

  • Hi RuihW,

    isn't it sufficient to simply send your expression to Calculator, correct any syntax erorrs, and then press "Evaluate the buffer" to get the result you are interested in? Or do you actually need it in your result list, e.g. for automatically generating a datasheet?

    Of course, if you have to correct any syntax errors, I don't see how your original expression should get updaed, as it then contains a different expression.

    But I sometimes noticed the effect, that if you add a new expression AFTER simulation is complete (and probably also AFTER having it evaluated once by Calculator), by using the "Send buffer expression to ADE Outputs" buttton, then the expression is added AND the value is also there (but only for a single point simulation). Maybe this helps?

  • Hi RuihW, 

    For the first part of your question, yes, it is possible to change your expressions and re-evaluate the modified output to get new results without having to re-run. This can be done using the Plot Outputs button located on the Run toolbar in ADE Explorer. After updating your expressions in the output set, kindly click on the Plot Outputs button to start the re-evaluations. Once done, you should see the new results and signal plots. If you do not want to see the plots but only expression updates, it might be a good idea to disable the plot on the signals before the re-evaluation. 

    For your last question, from my understanding and the messages given, I will say yes, Spectre had a convergence issue with the gmin homotopy method. The simulator uses different continuation methods to help with convergence. As a result, it uses one method at a time, and when that fails, it moves to the next method in a particular order, starting with gmin. However, you can set the method to use manually in your simulation. To do this, go to Simulation => Options => Analog => Alogarithm Tab, and under the Convergence Options, you can select the homotopy method to use. In your case, you can choose source and then click Ok.  Thank you 

  • in reply to Volker T

    Thanks Volker. I'll try the calculator. There are about 6500 expressions to be evaluated, but they all have the same format. So hopefully I can get them all updated from the calculator by some SKILL scripts.

  • in reply to Seiba

    Thanks Seiba! This is exactly what I'm looking for.

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.