Exporting/plotting data w/ constant time step in IC6.1.5

 Is there really no solution to this? I can use the ahdl "sample" to export data to a file, but that is a bit of a pain.

Does anyone know how to get the sample() function working with the new calculator?

Yes, there's a solution - personally I didn't reply because I've been busy with the day job (we're all volunteers on this forum, including the Cadence folks - we do this in our spare time).

First of all, I suspect you're using an early version of IC615 (either the base release, or an early hotfix). The table wasn't ready, and we didn't want to provide the Java table that had been in previous releases, so it temporarily reverted to the old ADE "print engine" which is a little limited.

From IC615 ISR6 (I think it was ISR6) there's a new table. The new table can plot the entire waveform to the table, and once in there you can do RMB->Sample to sample it to a regular grid.

1. It shouldn't do that any more after ISR6
2. No idea why the sample() function is giving that error - I doubt it's the sample function that's saying that, since your expression should work fine (I tried it).
3. If you want ocnPrint to output on a regular timestep you can use the optional ?from ?to and ?step arguments to ocnPrint . See the documentation for more information
4.  I just tried that, and got no error. I cannot see why you should get an error from this.

You might want to post the precise error you're getting for 2 and 4, as well as the subversion you're using. I'd try a later hotfix anyway though.

You might also want to look at the strobeperiod option on transient - this means that the simulator will solve and output on a regular grid - it may take more timesteps internally and not output them. The benefit of this approach is that it eliminates interpolation error, which is good if you're wanting to DFT the results (assuming you are on the same grid).

Regards,

Andrew.

 Thanks Andrew. I'll try those and report back.

Andrew - sorry it took so long but I still can't get it to work. Here is the error when I try something simple, like trying to plot using the sample() function.

Any ideas?

Rob,

I've figured out what the problem is. Somebody has defined a SKILL function called value() in your environment, and that is being used instead of the standard Cadence value() function.

I can reproduce the same problem if I do:

procedure(value() t)

The message about value in your screenshot is the clue - it says too many arguments, 0 expected. If I do arglist('value) it should show:

(wave \@key scale period xName
    histoDisplay
    (noOfHistoBins 1) \@rest args
)

So you need to find where this local value() function is being defined, and remove that. Maybe running with "virtuoso -nocdsinit" as a short term solution might help. If you have the SKILL development environment available, you could start with -nocdsinit, then do:

installDebugger()
load(".cdsinit")  ; you might need to give the right path to the .cdsinit to make sure you pick up the right one

Then afterwards  (assuming it's all loaded OK and the problem remains), type whereIs(value) - it should tell you which file the modified value() function came from (it has to be done with the debugger enabled).

This is precisely the reason why we advise that customer SKILL code should be written using a unique prefix for each function, ideally starting with uppercase to avoid clashing with Cadence-supplied functions.

Regards,

Andrew.

 Thanks for all the work on this Andrew. I'm trying to verify if someone did create that function.