I am simulating an ADC in the goal to calculate the FFT.I am using a sine wave as an input(Fin=10Khz). Each conversion takes 6.5us and I would like to run for 6.7ms. Fsampling=154KhzI am using the spectreS simulator and now, the simulation takes at least 2 days and more.Does anyone know how to fix the step in the order to get faster simulation ?
Thanks for your help !!!
Why are you using the spectreS interface to spectre? It's old and has been end-of-lifed for several years (in fact it no longer exists in releases after IC5141). Ideally you should use the "spectre" interface, as this is being maintained and is a more direct interface to the simulator. Which subversion of DFII are you using (Help->About in the CIW), and which version of spectre are you using (this will appear in the output log, or by typing "spectre -W" at the UNIX prompt)?
You cannot have fixed step sizes with spectre; you can use things like strobeperiod to write out with a regular step, but the simulator will still take smaller steps internally if needed in order to follow the waveforms. Taking fixed size steps in a circuit simulator would be a mistake because you are then potentially not following the signals accurately enough.
First thing I would check is whether the simulator is taking very short timesteps - you should be able to check this from the log file. If so, are you specifying excessively tight rise/fall times on your pulse/pwl sources? The simulator will have to try to follow them if you do, and it then takes time to relax the timestep after each edge. Perhaps your device models have discontinuities, and it could be exacerbated by using non-physical inductor/capacitor values in your circuit, leading to instability (which has to be followed). Sometimes using the cmin option on the tran analysis can help by adding a small capacitor to every node to damp things a little.
You could (if you were using spectre rather than spectreS) use either spectre turbo, or APS (assuming your licenses are recent enough, and you have a new enough simulator release, and a new enough IC5141 version) to gain further acceleration. Very hard to tell without more information...
In reply to Andrew Beckett:
Thanks for your response,
I am using this version of spectre: sub-version 188.8.131.52808
I am trying to do a long simulation like 6.6ms. After 976.254us, i got this message.
Error found by spectre at time = 976.254 us during transient analysis `tran'. SST2 Error: No space left on deviceAnalysis `tran' terminated prematurely due to error.finalTimeOP: writing operating point information to rawfile.Trying `homotopy = gmin'.Trying `homotopy = source'.Trying `homotopy = dptran'.
Error found by spectre during info `finalTimeOP'. Unable to start type table in the PSF file `finalTimeOP.info'.
Error found by spectre during info `modelParameter'. Unable to start type table in the PSF file `modelParameter.info'.
Do you have any idea ?
Thanks for your help
In reply to Riccart07:
In reply to Hasan AA:
Hasan AAHello, I have the same question. I am using some verilog-A block and it takes huge time for the simulation. I was wondering if there is anyway to improve the speed simulation!