Stats

  • Locked Locked
  • Replies 3
  • Subscribers 125
  • Views 22465
  • 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

Setting TimeStep for Transient simulations : defaulting to ps

HariV

I'm tying to test my design using MATLAB.  Specifically, I'm exporting time domain simulation data into MATLAB to do FFT in MATLAB.

FFT requires coherently sample data.  Therefore, my time domain data needs precise time step.  For instance, for a sampling frequency of 50MHz, my time step must be 20ns. 

I tried setting this in ADE-> transient simulation options window. However, for some reason, the time step defaults to ~ps. 

Is there anyway I can set a time step in CADENCE and expect the same timestep in the simulation data?

Parents

  • Dear Hariv,

    I believe you need to set strobeperiod to your sampling period  in the transient analysis panel . If you only want the data at the strobeperiods (and not any intevervening time points, you might also consider setting strobeoutput=strobeonly.

    These are documented in both spectre -h and the Spectre Circuit Simulator Reference manual.

    Shawn

  • in reply to ShawnLogan

    To clarify this since you asked a similar question in a very old thread, it's on the transient options form - click Options on Transient and then you'll find it:

    The strobeoutput that Shawn mention defaults to strobeonly so you don't need to set that. Only if you want the strobe points and the other time steps found by the simulator do  you need to change this - e.g. to all.

    When this is set, the simulator ensures that it solves at the designated strobe time points, which eliminates accuracy issues caused by interpolation if you were to sample the data (e.g using the sample or dft functions in the calculator). That's normally only an issue if you're sampling non-settled data (i.e. at each sample point the signal is still changing), but it can certainly improve accuracy.

    Why are you doing an FFT in Matlab? You can use the dft function in the calculator to perform an FFT, and since IC617 this no longer requires a power of 2 number of samples (before it rounded to a power of 2).

    Regards,

    Andrew.

  • in reply to Andrew Beckett

    Thank you, Andrew, for taking your valuable time to provide greater detail, and more importantly, making the response much more valuable for HariV and others!

    Shawn

Reply Children
No Data

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.