The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> Wavescan Waveform viewer & Calculator
https://designers-guide.org/forum/YaBB.pl?num=1108170141

Message started by kmjoshi on Feb 11^th, 2005, 5:02pm

Title: Wavescan Waveform viewer & Calculator
Post by kmjoshi on Feb 11^th, 2005, 5:02pm

Hello,

I am using "Spectrespp " (Spectre in text format) to run a SPICE file.
I am using the "wavescan" waveform viewer tool to view the waveforms.

Since my simulations take a long time, if I do not mention anything, spectre saves the waveforms at all the nodes. This occupies a lot of space on the hard disk.

Is there any way I could tell it to plot only the waveforms I want.

I know the use of .PLOT command plots the nodes I tell it to but at the same time it plots other waveforms too.

How do I save disk space as the .raw files occupy a lot of space?

One another question, how do I use the Calculator in Spectre to integrate a waveform from one time limit to the other?

I know i could use integ but how do I give it the limits?

Thanks in advance for your help. :)

Regards,
Kirti

Title: Re: Wavescan Waveform viewer & Calculator
Post by Ken Kundert on Feb 11^th, 2005, 5:30pm

To control which waveforms are saved, use the save command and the save option.

-Ken

Title: Re: Wavescan Waveform viewer & Calculator
Post by Andrew Beckett on Feb 11^th, 2005, 11:14pm

If you use IC5141 you can avoid having to use spp to preprocess the data. If you use "spectre +csfe input.ckt" it will parse the SPICE syntax netlist natively. If you use the later MMSIM60 release of spectre, then the new front end (which is what +csfe enables) is on by default.

To do what Ken says, you'd then put this in your netlist:

Code:

simulator lang=spectre
save node1 node2 node3
simulator lang=spice

The simulator lang= is needed if the file is not in spectre syntax, or if the file does not have a .scs suffix (.scs implies spectre language mode).

As for the wavescan question, then if you are using wavescan standalone, you have two choices:

1. You can use Settings->Select Data in the results browser window. This will allow you to specify the start and end points as the data is read in (in other words it doesn't even read the data outside these ranges, saving memory). The same menu can be used with swept data to pick the parameter sweep values you want to read.
2. Perhaps a more likely way - use the "trim" function in the calculator.

If you're using wavescan in ADE (in IC5141 or later), then the calculator functions are then not using spectreMDL, but SKILL, and so the calculator function would be "clip". Rather confusingly wavescan standalone has a function "clip" which does clipping in the Y direction (a more sensible name, really).

Regards,

Andrew.