Can't understand this error in IC610

[som...@yahoo.com]

Hi,

I'm trying to plot the gsd parameter of a MOS transistor during DC
sweep. I have done "save M:oppoint" and simulation goes ok. Then from
results browser I'm able to plot gds vs. the sweep parameter in
wavescan. What I wanted to do next was to input this waveform in
calculator, do some processing, namely invert it and plot again. While
I try to plot it from calculator though, I get the following error:

- Warning -
<Calculator>
Evaluation error(ERROR : ("quotient" 0 t nil ("*Error* quotient:
can't handle (1 / nil)"))). Expression: 1/getData("/MN:gds" ?
resultsDir "/home/simulation/HW4_pr3/spectre/schematic" ?result "dc-
dc")

- Warning -
<Calculator>
Evaluation error(Unknown scalar data type: nil). Expression: getData
("/MN:gds" ?result "dc-dc")

As far as I understand it, it says that the denominator is 0 (nil).
However, I just got it from wavescan, so it can't be nil. Even if I
try to put it in the calculator and plot from there, without any
processing it still gives the same error. I tried doing the same
procedure on a regular AC analysis, just plotting node voltages from
results browser and from calculator. It works without a problem. Can
anyone help, please? Thanks

[Tarek]

one way around this is to plot gds in wavescan, open calculator,
select wave, click on the waveform in wavescan, then change the
calculator expression to 1/waveXY() then plot that. however that won't
work if you want to make than an output in ADE. i'm sure there's a
better way.

[Tarek]

I just looked a bit closer at your save statement. Try "save
M*:oppoint", or simply "save *:oppoint". refer to "spectre -h save"
for options.

[som...@yahoo.com]

Thank you for your replies. Unfortunately I don't think it is really a
problem of how one defines the save oppoint. Because with the way I do
it I have no problems seeing the gds curve in wavescan - so, it
extracts the data from the DC sweep. It is just that when I try to put
it in the calculator and then plot back in wavescan, that it kind of
"loses" it. But I'll try what you recommended.

[Andrew Beckett]

som...@yahoo.com wrote, on 10/20/09 18:16:

Try changing the getData("/MN:gds"...) to getData("MN:gds"). I suspect something
is getting confused about the mapping of device names. Names which begin with
"/" are schematic names, whereas those without are "simulator" names. So
providing you use the names in the netlist, all should be OK.

You might also want to try pv("/MN" "gds" ?result "dc-dc") - but I'm guessing a
bit here.

Either way, it shouldn't really be getting this wrong, so you might want to
contact Cadence customer support to investigate why the mapping is going wrong.
There might be something afoot with the CDF for your transistors (maybe).

Regards,

Andrew.

[som...@yahoo.com]

Hi Andrew,

Removing "/" actually worked. Thanks a lot.
The second thing you suggested didn't help, but who cares, as long as
I have a working solution.