PSpice worst case simulation

I even sent him a detailed treatise from IntuSoft, but I fear that Joerg has no experience rolling his own models. He needs to practice up on making subcircuits and behavioral things... hone up his math ;-)

I can't even fathom a large enough number to count all the models I've made. I'm fond of making my own tool devices... that automatically do all the things that LTspice calls up as "Measure"... my tools display the results in Probe :-) ...Jim Thompson

Oh, I've made models in the past. Just not opamps, and not with a pounding flu-infested head like right now ;-)

Maybe I just place a voltage source in front of every opamp and let it step the voltage. I can already hear the comments ... "GAAAAAH" ... and ... "EEEUW" ... :-)

Nothing generally wrong with that. But I always have to wonder about designs where +/-7mV VOS would be an issue ;-) ...Jim Thompson

I am quite sure it won't be. But the task at hand is to provide proof that it won't be ;-)

Trust me ;-) ...Jim Thompson

To keep it pretty (and invisible to the client), put the voltage source inside the subcircuit. Parameterize the value of VOS, but do it global so you can manipulate from outside. ...Jim Thompson

It's a design by the client, and they are very professional guys. At the end they should see everything that is in the sims so they can talk it over.

I'll probably have to do the params thing on a voltage source or something. But first I want to ask Cadence support whether there isn't a secret hook to unlock the real-world sim. I mean, what's the point of even having an offset in the model (and this one does) when the simulator then blindly takes a 7mV entry as always being +7mV and ignores PTOL and NTOL completely. If you enter -2mV it always calculates with -2mV. To me that makes no sense in a worst case sim. If, as Charlie assumes, this feature is only available by forking over some more bucks then at least PSpice should respond with a stop sign or "not available at this level".

Using the roached on voltage sources right now. Found out another thing tho: WC does not like math expressions for the output variable, such as ABS(V(yadayada)). It errors on that. Oh man. Ok, I can make a kludge for that as well but I must say this is all a bit disappointing. Looks like in the end I'll have a sim with two dozen kludges, a couple of car jacks, five shims and 10ft of duct tape.

I haven't used in a very long time. What error message? The correct format, if allowed, would be...

{abs(V(yadyadadoo))}

Note the curly brackets. ...Jim Thompson

Result remains as usual:

.WCASE TRAN {ABS(V(PORTLEFT-L))} YMAX VARY DEV HI

------------$ ERROR -- Invalid Expression: Specify either current(I) or voltage(V) or digital(D).

Jamie, same for your version :-(

Ok, maybe PSpice really can't do that (which would be sad), but if it somehow can, what's so difficult about having a more intuitive user interface? It could say "Expression "xxxyyxx" errored, did you mean "xxxyxx" instead?". Better yet they should keep nomenclature consistency between probe and other parts of the program. Because the probe window eats and displays it properly, without curly brackets.

Guess another band aid is needed, an ideal rectifier or a behavioral thingamagic with a voltage output. More duct tape :-)

How about wrapping the OpAmp model within a parameterized model with the appropriate offset sources?

Sonnova gun... there's a part called ABS ;-)

Although I wonder, is "PORTLEFT-L" a node name? Or did you mean subtraction? That would be V(PORTLEFT,L) Dashes aren't generally allowed in node names. ...Jim Thompson

they

Yes, that may be the only option. Beats me why they have all these parameter entries then. Unless VOS can be accessed by a MC or worst case sim it seems fairly meaningless to me, if you have to set it to zero and provide your own voltage source anyhow.

Did you try (ABS(V(xxxx))) ?

Jamie

Yup, in the function library, and it's in there now :-)

Band aids, band aids ...

It's a port name. Orcad picked it so I figured PSpice ought to eat it. But I'll name all that differently in the real thing. This was just a kicking the tires test.

Quick follow-up after receiving a response from support: Charlie was right, PSpice quietly ignores this stuff unless you buy a license for the advanced analysis package. So I'll just kludge voltage and current sources in there to get around this.