PSpice worst case simulation

[Joerg]

Hi Folks,

Reached an end of a rope here: How do you make a worst case simulation
in PSpice (or even Monte Carlo for that matter) properly find the
extremes for an opamp offset voltage and input bias current?

For example, for the opamp we have:

VOS: Offset voltage
VOS_DIST: Distribution, I assume
VOS_NTOL: What gets entered here?
VOS_PTOL: ... and here?

If I enter 7mV or whatever for VOS and set the distributuion to flat the
sim acts as if there was always +7mV. No variation. But we all know that
it'll be +/-7mV. How can I make PSpice understand that? The manual
appears to be silent about it and a web search doesn't even find
expressions such as VOS_NTOL.

Same goes for input bias current except that there it's called IB,
IB_DIST, IB_NTOL and IB_PTOL. Having to massage all these by hand gets
old in a larger simulation.

 

[Charlie E.]

Hi Folks,

Reached an end of a rope here: How do you make a worst case simulation
in PSpice (or even Monte Carlo for that matter) properly find the
extremes for an opamp offset voltage and input bias current?

For example, for the opamp we have:

VOS: Offset voltage
VOS_DIST: Distribution, I assume
VOS_NTOL: What gets entered here?
VOS_PTOL: ... and here?

If I enter 7mV or whatever for VOS and set the distributuion to flat the
sim acts as if there was always +7mV. No variation. But we all know that
it'll be +/-7mV. How can I make PSpice understand that? The manual
appears to be silent about it and a web search doesn't even find
expressions such as VOS_NTOL.

Same goes for input bias current except that there it's called IB,
IB_DIST, IB_NTOL and IB_PTOL. Having to massage all these by hand gets
old in a larger simulation.

Joerg,
Well, that should be
VOS: Offset voltage,
VOS_DIST: Distribution type, probably FLAT
VOS_NTOL: Negative tolerance
VOS_PTOL: Positive tolerance

So, if you wanted +/- 7mV, then VOS = 0, VOS_DIST = FLAT, VOS_NTOL =
7mv, VOS_PTOL = 7mv

At least, that is what I think it should be. Could be NTOL should be
-7mV...

Charlie

 

[Joerg]

Joerg,
Well, that should be
VOS: Offset voltage,
VOS_DIST: Distribution type, probably FLAT
VOS_NTOL: Negative tolerance
VOS_PTOL: Positive tolerance

So, if you wanted +/- 7mV, then VOS = 0, VOS_DIST = FLAT, VOS_NTOL =
7mv, VOS_PTOL = 7mv

At least, that is what I think it should be. Could be NTOL should be
-7mV...

I had already tried both. It no workie :-(

Looked around to find a description of this stuff but no dice either.
Maybe this is restricted to an inner circle of gurus who know the secret
knock on the back door ;-)

 

[Joerg]

First order of business... does your OpAmp MODEL support MC
parameterization?

For the test it's an LM324. I took it from the PSpice advanced analysis
directory and assume (but not sure) that PSpice should have sounded some
siren if it wasn't MC-ready and you run a MC. Plus it has all the entry
fields.

Confucius further says, "He who lives by Crapture, dies by Crapture"
;-)

But Confucius also say customer is king and if customer want Capture
then use Capture

 

[Joerg]

Did you read the IntuSoft reference I sent?

Yes, I read that and the others cover to cover. But VOS isn't described
in there. It describes how to do MC and worst case on LOT and DEV
variations in BJTs and so on. I only need to do worst case, plus MC as a
sanity check.

Did you take heed of my previous post... "First order of business...
does your OpAmp MODEL support MC parameterization?"

If it isn't parameterized in the model, you're dead in the water.

Ok, but how does one know? Why would it have a gazillion attribute
entries such as VOS_NTOL and VOS_PTOL if those can't be used? AFAIU
worst case and MC are the only sims that could use such information. I'd
expect PSpice to refuse entry if I tried entering data that isn't
supported by a model.

 

[Joerg]

None of the LM324 models I have on hand show DEV or LOT in the model
card. Can you post your model so I can see?

The LM324 model doesn't have DEV and LOT (I don't need both) but it does
have fields for high/low of the offset parameters and various others:

http://www.analogconsultants.com/ng/sed/LM324_pspice.jpg

If this model can't support MC or worst case, why would there even be
those Postol and Negtol fields? They appear to be editable because when
I change them the values stick.

 

[Joerg]

Crapture has changed the entry method for doing analysis.... obviously
not for the better

I just opened my copy of Crapture, v10.5i, so it's dated and likely
differs from yours...

Click on PSpice, Edit Simulation profile, Monte Carlo/Worst Case.

What do you have entered there?

That's still the same in 16.3. It is set to Monte Carlo, output variable
to output node of opamp, 10 runs, uniform distribution, save all data.

I also tried worst case, same thing, won't wiggle the opamp offset a
bit. It does work on resistors and stuff though. Although even there
PSpice is a bit odd because it only lets you find the min _or_ the max
of the output, but not both together in one plot. Doesn't make sense,
but then again it seems a few other things don't make much sense either.

 

[Joerg]

You've discovered my point... look at this model...

.MODEL N1 NPN (IS=5E-16 LOT/UNIFORM=90% DEV/GAUSS=3%)
+ BF=220 LOT/UNIFORM=50% DEV/GAUSS=2%)
+ BR=0.7 NR=1
+ ISE=3.5E-16 IKF=3E-3 IKR=3E-2 NE=1.4 NC=0.8 VAF=60
+ VAR=7 RC=15 RE=2 RB=200 RBM=100 IRB=3E-4 XTB=1.17
+ XTI=2.2 EG=1.235 TF=69.09E-12 TR=9E-9 XTF=0.3 VTF=6
+ ITF=5E-5 CJE=0.105E-12 MJE=0.8 VJE=0.8 ISC=1E-15
+ KF=2E-13 AF=1.4

Does your OpAmp model have those LOT and DEV entries?

No, it doesn't. Other opamps don't either, so far I only saw them in
discretes. Why would it need them if there are NTOL and PTOL entries?

 

[Charlie E.]

Yes, I read that and the others cover to cover. But VOS isn't described
in there. It describes how to do MC and worst case on LOT and DEV
variations in BJTs and so on. I only need to do worst case, plus MC as a
sanity check.



Ok, but how does one know? Why would it have a gazillion attribute
entries such as VOS_NTOL and VOS_PTOL if those can't be used? AFAIU
worst case and MC are the only sims that could use such information. I'd
expect PSpice to refuse entry if I tried entering data that isn't
supported by a model.

Joerg,
Don't know for sure, but those may be Advanced Analysis parameter,
only useful if you have the AA option for PSpice. They didn't sound
familiar to me from plain vanilla...

Charlie

 

[Charlie E.]

For the test it's an LM324. I took it from the PSpice advanced analysis
directory and assume (but not sure) that PSpice should have sounded some
siren if it wasn't MC-ready and you run a MC. Plus it has all the entry
fields.



But Confucius also say customer is king and if customer want Capture
then use Capture

Ok, I bet you don't have Advanced Analysis, or if you do, you aren't
using the Advanced Analysis menu to do the WC and MC sims. They are
in a different place than the regular menus in the simulation profile!

Charlie

 

[Joerg]

If they're not in the model....

But then why wouldn't those fields be grayed out or refusing entries in
the simulator? I can enter data there and it sticks, meaning after
saving it's still there.

Why aren't you watching "Dances"? I'm on a commercial break

Oh, I was. But on the couch and half dozed off. Caught some sort of flu
bug :-(

This season there are some really good candidates, lots of talent. And
Bruno is promising to live up to his usual exuberant outbursts pretty soon.

 

[Joerg]

Joerg,
Don't know for sure, but those may be Advanced Analysis parameter,
only useful if you have the AA option for PSpice. They didn't sound
familiar to me from plain vanilla...

Yes, that's what I am afraid may be true. I'll open a support ticket
then, to find out for sure. I just wonder, what good would it do if they
provide worst case analysis in the regular PSpice and then you can't
scoot an offset for tolerance?

 

[Joerg]

Ok, I bet you don't have Advanced Analysis, or if you do, you aren't
using the Advanced Analysis menu to do the WC and MC sims. They are
in a different place than the regular menus in the simulation profile!

I don't have the license for Advanced. But the menu items I described
where in regular PSpice. They just don't do anything there.

 

[Charlie E.]

Yes, that's what I am afraid may be true. I'll open a support ticket
then, to find out for sure. I just wonder, what good would it do if they
provide worst case analysis in the regular PSpice and then you can't
scoot an offset for tolerance?

To be honest, it all depends on the models. Most opamp models don't
have those variable set up to tolerance offsets, etc. The AdvAnal
models were custom made to be able to add in all those extras, to
justify some of the added expense of the option!

You can always modify the existing models to add those tolerances. Jim
gave you a few clues on how to do that.

Charlie

 

[Joerg]

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 ;-)

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

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

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" ...

 

[Joerg]

I don't quite know how this "advanced" stuff is supposed to work,
but you can still do MC and WC... just modify your models as I noted
previously.

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.

 

[Joerg]

[snip]
I don't have the license for Advanced. But the menu items I described
where in regular PSpice. They just don't do anything there.
I don't quite know how this "advanced" stuff is supposed to work,
but you can still do MC and WC... just modify your models as I noted
previously.

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.

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

 

[Jamie]

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.

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

Jamie

 

[Joerg]

Jim Thompson wrote:
[snip]
I don't have the license for Advanced. But the menu items I described
where in regular PSpice. They just don't do anything there.
I don't quite know how this "advanced" stuff is supposed to work,
but you can still do MC and WC... just modify your models as I noted
previously.

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.

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

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

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

Band aids, band aids ...

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.

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.

 

[Joerg]

Hi Folks,

Reached an end of a rope here: How do you make a worst case simulation
in PSpice (or even Monte Carlo for that matter) properly find the
extremes for an opamp offset voltage and input bias current?

For example, for the opamp we have:

VOS: Offset voltage
VOS_DIST: Distribution, I assume
VOS_NTOL: What gets entered here?
VOS_PTOL: ... and here?

If I enter 7mV or whatever for VOS and set the distributuion to flat the
sim acts as if there was always +7mV. No variation. But we all know that
it'll be +/-7mV. How can I make PSpice understand that? The manual
appears to be silent about it and a web search doesn't even find
expressions such as VOS_NTOL.

Same goes for input bias current except that there it's called IB,
IB_DIST, IB_NTOL and IB_PTOL. Having to massage all these by hand gets
old in a larger simulation.

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.