significant digits in ADE assembler output expressions

You can control the output precision either using Options->Output Formatting or per-output using this column:

I'm slightly surprised though that if you have expressions used in other expressions as dependencies, then I wouldn't expect the truncation to have occurred (It's really just a display thing). Maybe it's become a fixed number at some point - it's not entirely clear what your setup looks like.

Andrew

Thanks for your reply, Andrew. Perhaps I haven't made myself clear enough. I mean that the values in the expression itself, instead of the values of the expressions' results, has been truncated. It seems that the 'Digits' column or Output Formatting only applies to the latter one.

below is how I set up my expressions:

First I plot spectrum using "Measurements"-"Spectrum" in ViVa. Then I select the spectrum waveform and send it to Calculator, where I got the expression "db20(dft((VT("/VXP") - VT("/VXN"))  1.989955e-06 22.469955u 1024 "Rectangular" 0 0 1))". The start and stop time is exactly what I want.

Then, I select the spectrum waveform and send it to ADE. In ADE I found that the expression has become "db20(dft((VT("/VXP") - VT("/VXN")) 1.989955e-06 2.246996e-05 1024 "Rectangular" 0 0 1))". The stop time is now 2.246996e-05 (22.46996u instead of 22.469955u). I try to set stop time to 2.2469955e-05 manually, but it just doesn't work. I believe it isn't just a display thing, since as I re-evaluated the results in ADE, I do see spectrum leakage (which indicates that the FFT time window has changed).

Something's wrong when I tried to upload screenshots :( I hope my descriptions are clear enough.

I can reproduce the problem. I found a workaround which preserves the precision of the numbers with 8 significant digits but it's not robust - and I don't think it is a clean way of doing this. I'll file a CCR to try to address this properly.

The best solution for now is to ensure that you have variables (design variables for example) instead of the literal numbers in the expression. For example, if I use:

(note I have changed the literal numbers to be VAR() expressions) then it works reliably. I used the same variables in the transient analysis too to ensure that the simulator strobes at the same times as the dft is sampling at (skipstart, strobeperiod and strobeoutput). I'll try appending that separately.

Andrew

Oh, I can't upload the picture (same problem you had). I set (on the tran options form):

skipstart : tsampstart
sprobeperiod: tstep
strobeoutput: all

(the last just means you get all the points, not just those where the simulator has strobed at). This tends to reduce the numerical noise floor of the DFT (unnecessary if the sample points are fully settled and don't need to interpolate).

Andrew

Oh, I can't upload the picture (same problem you had). I set (on the tran options form):

skipstart : tsampstart
sprobeperiod: tstep
strobeoutput: all

(the last just means you get all the points, not just those where the simulator has strobed at). This tends to reduce the numerical noise floor of the DFT (unnecessary if the sample points are fully settled and don't need to interpolate).

Andrew