PSpice worst case simulation

Started by Joerg March 21, 2011
On Tue, 22 Mar 2011 15:42:36 -0700, Joerg 
wrote:

>Jim Thompson wrote: >> On Tue, 22 Mar 2011 10:51:26 -0700, Joerg >> 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. ...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 Tue, 22 Mar 2011 15:42:36 -0700, Joerg > wrote: > >> Jim Thompson wrote: >>> On Tue, 22 Mar 2011 10:51:26 -0700, Joerg >>> 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 :-) -- Regards, Joerg http://www.analogconsultants.com/ "gmail" domain blocked because of excessive spam. Use another domain or send PM.
On Tue, 22 Mar 2011 13:31:11 -0700, Joerg  wrote:

>Jim Thompson wrote: >> On Tue, 22 Mar 2011 12:54:35 -0700, Joerg >> wrote: >> >>> Jim Thompson wrote: >>>> On Tue, 22 Mar 2011 12:43:19 -0700, Joerg >>>> wrote: >>>> >>>>> Jim Thompson wrote: >>>>>> On Tue, 22 Mar 2011 11:58:51 -0700, Charlie E. >>>>>> wrote: >>>>>> >>>>>>> On Tue, 22 Mar 2011 10:49:21 -0700, Joerg >>>>>>> wrote: >>>>>>> >>>>>>>> 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 >>>>>> 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" ... :-) >>>> Nothing generally wrong with that. But I always have to wonder about >>>> designs where +/-7mV VOS would be an issue ;-) >>>> >>> I am quite sure it won't be. But the task at hand is to provide proof >>> that it won't be ;-) >> >> 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. >> > >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".
How about wrapping the OpAmp model within a parameterized model with the appropriate offset sources?
On Tue, 22 Mar 2011 16:23:59 -0700, Joerg 
wrote:

>Jim Thompson wrote: >> On Tue, 22 Mar 2011 15:42:36 -0700, Joerg >> wrote: >> >>> Jim Thompson wrote: >>>> On Tue, 22 Mar 2011 10:51:26 -0700, Joerg >>>> 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 ;-) 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 -- | 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
krw@att.bizzzzzzzzzzzz wrote:
> On Tue, 22 Mar 2011 13:31:11 -0700, Joerg wrote: > >> Jim Thompson wrote: >>> On Tue, 22 Mar 2011 12:54:35 -0700, Joerg >>> wrote: >>> >>>> Jim Thompson wrote: >>>>> On Tue, 22 Mar 2011 12:43:19 -0700, Joerg >>>>> wrote: >>>>> >>>>>> Jim Thompson wrote: >>>>>>> On Tue, 22 Mar 2011 11:58:51 -0700, Charlie E. >>>>>>> wrote: >>>>>>> >>>>>>>> On Tue, 22 Mar 2011 10:49:21 -0700, Joerg >>>>>>>> wrote: >>>>>>>> >>>>>>>>> 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 >>>>>>> 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" ... :-) >>>>> Nothing generally wrong with that. But I always have to wonder about >>>>> designs where +/-7mV VOS would be an issue ;-) >>>>> >>>> I am quite sure it won't be. But the task at hand is to provide proof >>>> that it won't be ;-) >>> 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. >>> >> 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". > > How about wrapping the OpAmp model within a parameterized model with the > appropriate offset sources?
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. -- Regards, Joerg http://www.analogconsultants.com/ "gmail" domain blocked because of excessive spam. Use another domain or send PM.
Jim Thompson wrote:
> On Tue, 22 Mar 2011 16:23:59 -0700, Joerg > wrote: > >> Jim Thompson wrote: >>> On Tue, 22 Mar 2011 15:42:36 -0700, Joerg >>> wrote: >>> >>>> Jim Thompson wrote: >>>>> On Tue, 22 Mar 2011 10:51:26 -0700, Joerg >>>>> 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. -- Regards, Joerg http://www.analogconsultants.com/ "gmail" domain blocked because of excessive spam. Use another domain or send PM.
Joerg 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. >
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. -- Regards, Joerg http://www.analogconsultants.com/ "gmail" domain blocked because of excessive spam. Use another domain or send PM.
Jim Thompson wrote:
> On Mon, 21 Mar 2011 16:46:05 -0700, Joerg > wrote: > >> Charlie E. wrote: >>> On Mon, 21 Mar 2011 16:10:43 -0700, Joerg >>> 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. -- Regards, Joerg http://www.analogconsultants.com/ "gmail" domain blocked because of excessive spam. Use another domain or send PM.
On Mon, 21 Mar 2011 16:46:05 -0700, Joerg 
wrote:

>Charlie E. wrote: >> On Mon, 21 Mar 2011 16:10:43 -0700, Joerg >> 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? 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. ...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 16:10:43 -0700, Joerg > 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 :-) -- 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 16:10:43 -0700, Joerg > 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 ;-) -- Regards, Joerg http://www.analogconsultants.com/ "gmail" domain blocked because of excessive spam. Use another domain or send PM.
On Mon, 21 Mar 2011 16:10:43 -0700, Joerg 
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? Confucius further says, "He who lives by Crapture, dies by Crapture" ;-) ...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 16:10:43 -0700, Joerg 
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... Charlie
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.

-- 
Regards, Joerg

http://www.analogconsultants.com/

"gmail" domain blocked because of excessive spam.
Use another domain or send PM.