Forums

PSpice worst case simulation

Started by Joerg March 21, 2011
Jim Thompson wrote:
> On Mon, 21 Mar 2011 17:47:14 -0700, Joerg <invalid@invalid.invalid> > wrote: > >> Jim Thompson wrote: >>> On Mon, 21 Mar 2011 17:07:27 -0700, Joerg <invalid@invalid.invalid> >>> wrote: >>> >>>> Jim Thompson wrote: >>>>> On Mon, 21 Mar 2011 16:46:05 -0700, Joerg <invalid@invalid.invalid> >>>>> wrote: >>>>> >>>>>> Charlie E. wrote: >>>>>>> On Mon, 21 Mar 2011 16:10:43 -0700, Joerg <invalid@invalid.invalid> >>>>>>> wrote: >>>>>>> >>>>>>>> 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... >>>>>>> >>>>>> 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 ;-) >>>>> 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. >>> 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. > > 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. -- Regards, Joerg http://www.analogconsultants.com/ "gmail" domain blocked because of excessive spam. Use another domain or send PM.
On Mon, 21 Mar 2011 18:37:23 -0700, Joerg <invalid@invalid.invalid>
wrote:

>Jim Thompson wrote: >> On Mon, 21 Mar 2011 17:47:14 -0700, Joerg <invalid@invalid.invalid> >> wrote: >> >>> Jim Thompson wrote: >>>> On Mon, 21 Mar 2011 17:07:27 -0700, Joerg <invalid@invalid.invalid> >>>> wrote: >>>> >>>>> Jim Thompson wrote: >>>>>> On Mon, 21 Mar 2011 16:46:05 -0700, Joerg <invalid@invalid.invalid> >>>>>> wrote: >>>>>> >>>>>>> Charlie E. wrote: >>>>>>>> On Mon, 21 Mar 2011 16:10:43 -0700, Joerg <invalid@invalid.invalid> >>>>>>>> wrote: >>>>>>>> >>>>>>>>> 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... >>>>>>>> >>>>>>> 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 ;-) >>>>>> 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. >>>> 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. >> >> 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.
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? ...Jim Thompson -- | James E.Thompson, CTO | mens | | Analog Innovations, Inc. | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | Phoenix, Arizona 85048 Skype: Contacts Only | | | Voice:(480)460-2350 Fax: Available upon request | Brass Rat | | E-mail Icon at http://www.analog-innovations.com | 1962 | Remember: Once you go over the hill, you pick up speed
Jim Thompson wrote:
> On Mon, 21 Mar 2011 18:37:23 -0700, Joerg <invalid@invalid.invalid> > wrote: > >> Jim Thompson wrote: >>> On Mon, 21 Mar 2011 17:47:14 -0700, Joerg <invalid@invalid.invalid> >>> wrote: >>> >>>> Jim Thompson wrote: >>>>> On Mon, 21 Mar 2011 17:07:27 -0700, Joerg <invalid@invalid.invalid> >>>>> wrote: >>>>> >>>>>> Jim Thompson wrote: >>>>>>> On Mon, 21 Mar 2011 16:46:05 -0700, Joerg <invalid@invalid.invalid> >>>>>>> wrote: >>>>>>> >>>>>>>> Charlie E. wrote: >>>>>>>>> On Mon, 21 Mar 2011 16:10:43 -0700, Joerg <invalid@invalid.invalid> >>>>>>>>> wrote: >>>>>>>>> >>>>>>>>>> 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... >>>>>>>>> >>>>>>>> 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 ;-) >>>>>>> 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. >>>>> 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. >>> 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. > > 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? -- Regards, Joerg http://www.analogconsultants.com/ "gmail" domain blocked because of excessive spam. Use another domain or send PM.
On Mon, 21 Mar 2011 18:52:39 -0700, Joerg <invalid@invalid.invalid>
wrote:

>Jim Thompson wrote: >> On Mon, 21 Mar 2011 18:37:23 -0700, Joerg <invalid@invalid.invalid> >> wrote: >> >>> Jim Thompson wrote: >>>> On Mon, 21 Mar 2011 17:47:14 -0700, Joerg <invalid@invalid.invalid> >>>> wrote: >>>> >>>>> Jim Thompson wrote: >>>>>> On Mon, 21 Mar 2011 17:07:27 -0700, Joerg <invalid@invalid.invalid> >>>>>> wrote: >>>>>> >>>>>>> Jim Thompson wrote: >>>>>>>> On Mon, 21 Mar 2011 16:46:05 -0700, Joerg <invalid@invalid.invalid> >>>>>>>> wrote: >>>>>>>> >>>>>>>>> Charlie E. wrote: >>>>>>>>>> On Mon, 21 Mar 2011 16:10:43 -0700, Joerg <invalid@invalid.invalid> >>>>>>>>>> wrote: >>>>>>>>>> >>>>>>>>>>> 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... >>>>>>>>>> >>>>>>>>> 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 ;-) >>>>>>>> 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. >>>>>> 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. >>>> 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. >> >> 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?
If they're not in the model.... Why aren't you watching "Dances"? I'm on a commercial break :-) ...Jim Thompson -- | James E.Thompson, CTO | mens | | Analog Innovations, Inc. | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | Phoenix, Arizona 85048 Skype: Contacts Only | | | Voice:(480)460-2350 Fax: Available upon request | Brass Rat | | E-mail Icon at http://www.analog-innovations.com | 1962 | Remember: Once you go over the hill, you pick up speed
On Mon, 21 Mar 2011 17:07:27 -0700, Joerg <invalid@invalid.invalid>
wrote:

>Jim Thompson wrote: >> On Mon, 21 Mar 2011 16:46:05 -0700, Joerg <invalid@invalid.invalid> >> wrote: >> >>> Charlie E. wrote: >>>> On Mon, 21 Mar 2011 16:10:43 -0700, Joerg <invalid@invalid.invalid> >>>> wrote: >>>> >>>>> 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... >>>> >>> 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 ;-) >> >> 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, 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
On Mon, 21 Mar 2011 16:49:38 -0700, Joerg <invalid@invalid.invalid>
wrote:

>Jim Thompson wrote: >> On Mon, 21 Mar 2011 16:10:43 -0700, Joerg <invalid@invalid.invalid> >> wrote: >> >>> 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. >> >> 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 :-)
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
Jim Thompson wrote:
> On Mon, 21 Mar 2011 18:52:39 -0700, Joerg <invalid@invalid.invalid> > wrote: > >> Jim Thompson wrote: >>> On Mon, 21 Mar 2011 18:37:23 -0700, Joerg <invalid@invalid.invalid> >>> wrote: >>> >>>> Jim Thompson wrote: >>>>> On Mon, 21 Mar 2011 17:47:14 -0700, Joerg <invalid@invalid.invalid> >>>>> wrote: >>>>> >>>>>> Jim Thompson wrote: >>>>>>> On Mon, 21 Mar 2011 17:07:27 -0700, Joerg <invalid@invalid.invalid> >>>>>>> wrote: >>>>>>> >>>>>>>> Jim Thompson wrote: >>>>>>>>> On Mon, 21 Mar 2011 16:46:05 -0700, Joerg <invalid@invalid.invalid> >>>>>>>>> wrote: >>>>>>>>> >>>>>>>>>> Charlie E. wrote: >>>>>>>>>>> On Mon, 21 Mar 2011 16:10:43 -0700, Joerg <invalid@invalid.invalid> >>>>>>>>>>> wrote: >>>>>>>>>>> >>>>>>>>>>>> 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... >>>>>>>>>>> >>>>>>>>>> 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 ;-) >>>>>>>>> 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. >>>>>>> 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. >>>>> 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. >>> 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? > > 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. -- Regards, Joerg http://www.analogconsultants.com/ "gmail" domain blocked because of excessive spam. Use another domain or send PM.
Charlie E. wrote:
> On Mon, 21 Mar 2011 17:07:27 -0700, Joerg <invalid@invalid.invalid> > wrote: > >> Jim Thompson wrote: >>> On Mon, 21 Mar 2011 16:46:05 -0700, Joerg <invalid@invalid.invalid> >>> wrote: >>> >>>> Charlie E. wrote: >>>>> On Mon, 21 Mar 2011 16:10:43 -0700, Joerg <invalid@invalid.invalid> >>>>> wrote: >>>>> >>>>>> 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... >>>>> >>>> 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 ;-) >>> 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, > 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? -- Regards, Joerg http://www.analogconsultants.com/ "gmail" domain blocked because of excessive spam. Use another domain or send PM.
Charlie E. wrote:
> On Mon, 21 Mar 2011 16:49:38 -0700, Joerg <invalid@invalid.invalid> > wrote: > >> Jim Thompson wrote: >>> On Mon, 21 Mar 2011 16:10:43 -0700, Joerg <invalid@invalid.invalid> >>> wrote: >>> >>>> 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. >>> 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 :-) > > 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. -- Regards, Joerg http://www.analogconsultants.com/ "gmail" domain blocked because of excessive spam. Use another domain or send PM.
On Tue, 22 Mar 2011 10:51:26 -0700, Joerg <invalid@invalid.invalid>
wrote:

>Charlie E. wrote: >> On Mon, 21 Mar 2011 16:49:38 -0700, Joerg <invalid@invalid.invalid> >> wrote: >> >>> Jim Thompson wrote: >>>> On Mon, 21 Mar 2011 16:10:43 -0700, Joerg <invalid@invalid.invalid> >>>> wrote: >>>> >>>>> 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. >>>> 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 :-) >> >> 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.
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. ...Jim Thompson -- | James E.Thompson, CTO | mens | | Analog Innovations, Inc. | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | Phoenix, Arizona 85048 Skype: Contacts Only | | | Voice:(480)460-2350 Fax: Available upon request | Brass Rat | | E-mail Icon at http://www.analog-innovations.com | 1962 | Remember: Once you go over the hill, you pick up speed