# PSpice worst case simulation

Started by 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...
>>>>>>>
>>>>>>
>>>>>> 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...
>>>>>>>>
>>>>>>>
>>>>>>> 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/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...
>>>>>>>>>
>>>>>>>>
>>>>>>>> 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...
>>>>>>>>>>
>>>>>>>>>
>>>>>>>>> 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/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...
>>>>
>>>
>>> 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.
>>
>> 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...
>>>>>>>>>>>
>>>>>>>>>>
>>>>>>>>>> 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...
>>>>>
>>>>
>>>> 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.
>>> 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!
>

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.
>>>> 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!
>>
>
>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     |