Hello, I can run the simulation normally, but I haven’t been able to obtain the calculation results, and I would like to understand why.
For example, in the following case: when I set the simulation time from 14 ms to 15 ms and set the sampling time for each measurement to 14.9 ms to 15 ms, the post-processing outputs the results after the simulation ends.
However, when I shorten the simulation time to 4 ms to 5 ms and set the sampling time to 4.9 ms to 5 ms (at which point the circuit has already stabilized), the post-processing fails to produce any result.
I’ve tried many methods but still haven’t figured out the cause. For instance, when the simulation time is set from 9 ms to 10 ms, the results can be obtained if the number of parameter sets is 16. But when the number increases to 81, the results are no longer generated.
This inconsistent behavior—sometimes getting results and sometimes not—is quite frustrating. It’s especially disappointing to complete hundreds of simulations only to find that no results are produced.
I would really appreciate your advice. Thank you!
CirFile.txt (1.3 KB)
Beware that Qspice changed how time is saved if Tstart is included in .tran.
05/19/2025 T=0 is now set to the beginning of saving waveform data. To revert to the former behavior, add “.options ABSOLUTETIME”
Based on your netlist, it seems that you run .tran with Tstart at 4ms and Tstop at 5ms. Currently, in default, Qspice reset 4ms to 0s in its waveform data, therefore, in waveform data, time is just 0s to 1ms.
If you want Qspice to store data to begin and not to reset it time, you need this option
.option ABSOLUTETIME
Your waveform data will begin from Tstart when this is enable.
Your .meas always follow your waveform data… post-processing (.meas) is purely based on the output waveform data. Therefore, the time in .meas is refer to output waveform time axis. If you have Tstart, you have to pay extra attention. If you need everything in absolute time, add the option will help.
By the way, your .tran syntax is incorrect. This is Traditional Berkeley Syntax, 1st parameter is ignored. What your .tran (.TRAN 5m 4m 100n UIC) actually do is to ignore 5m, Tstop at 5m (Qspice take max of 1st and 2nd parameter as Tstop) and Tstart at 100n, UIC.
Correct version is .TRAN 0 5m 4m 100n UIC, where a 0 is added for ignored.
1 Like
Thank you very much for your suggestion!
It was very effective and helped me a lot.
Now I can confidently run large-scale parameter sweep simulations in QSPICE.
I truly appreciate your support once again.
1 Like
