Sign in

Not a member? | Forgot your Password?

Search Sci.Electronics.Design

Search tips

Recent Blogs on Electronics-Related

Two Capacitors Are Better Than One
posted by Jason Sachs


Voltage Drops Are Falling on My Head: Operating Points, Linearization, Temperature Coefficients, and Thermal Runaway
posted by Jason Sachs


Optimizing Optoisolators, and Other Stories of Making Do With Less
posted by Jason Sachs


Someday We’ll Find It, The Kelvin Connection
posted by Jason Sachs


10 Items of Test Equipment You Should Know
posted by Jason Sachs


First-Order Systems: The Happy Family
posted by Jason Sachs


Lost Secrets of the H-Bridge, Part IV: DC Link Decoupling and Why Electrolytic Capacitors Are Not Enough
posted by Jason Sachs


April is Oscilloscope Month: In Which We Discover Agilent Offers Us a Happy Deal and a Sad Name
posted by Jason Sachs


Specifying the Maximum Amplifier Noise When Driving an ADC
posted by Rick Lyons


BGA and QFP at Home 1 - A Practical Guide.
posted by Victor Yurkovsky


3 LEDs powered by fingers - puzzle
posted by Henryk Gasperowicz


Series circuit - 3 LEDs
posted by Henryk Gasperowicz


Video: The PN Junction. How Diodes Work?
posted by Stephane Boucher


Two jobs
posted by Stephane Boucher


2N3055 | 8051 | Amplifier | AVR | Battery | Capacitors | Charger | CMOS | Converter | DAC | Decoder | Demodulator | Diode | Ethernet | Flash | FPGA | GPS | I2C | IDE | Laser | LCD | LED | LTSpice | MOSFET | Op-amp | Oscillator | Oscilloscope | PCB | PID | PLL | PSpice | PSU | PWM | RFID | RS232 | RS485 | SMPS | Solenoid | Spice | Switcher | TCP/IP | Transformer | Transistor | TTL | USB | VCO | Zener

See Also

DSPEmbedded SystemsFPGA

design | PSpice worst case simulation


There are 37 messages in this thread.

You are currently looking at messages 31 to 37.

Re: PSpice worst case simulation - Jim Thompson - 2011-03-22 19:08:00

On Tue, 22 Mar 2011 15:42:36 -0700, Joerg <i...@invalid.invalid>
wrote:

>Jim Thompson wrote:
>> On Tue, 22 Mar 2011 10:51:26 -0700, Joerg <i...@invalid.invalid>
>> 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

Re: PSpice worst case simulation - Joerg - 2011-03-22 19:23:00

Jim Thompson wrote:
> On Tue, 22 Mar 2011 15:42:36 -0700, Joerg <i...@invalid.invalid>
> wrote:
> 
>> Jim Thompson wrote:
>>> On Tue, 22 Mar 2011 10:51:26 -0700, Joerg <i...@invalid.invalid>
>>> 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.

Re: PSpice worst case simulation - krw@att.bizzzzzzzzzzzz - 2011-03-22 19:37:00

On Tue, 22 Mar 2011 13:31:11 -0700, Joerg <i...@invalid.invalid> wrote:

>Jim Thompson wrote:
>> On Tue, 22 Mar 2011 12:54:35 -0700, Joerg <i...@invalid.invalid>
>> wrote:
>> 
>>> Jim Thompson wrote:
>>>> On Tue, 22 Mar 2011 12:43:19 -0700, Joerg <i...@invalid.invalid>
>>>> wrote:
>>>>
>>>>> Jim Thompson wrote:
>>>>>> On Tue, 22 Mar 2011 11:58:51 -0700, Charlie E. <e...@ieee.org>
>>>>>> wrote:
>>>>>>
>>>>>>> On Tue, 22 Mar 2011 10:49:21 -0700, Joerg <i...@invalid.invalid>
>>>>>>> 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? 

Re: PSpice worst case simulation - Jim Thompson - 2011-03-22 19:38:00

On Tue, 22 Mar 2011 16:23:59 -0700, Joerg <i...@invalid.invalid>
wrote:

>Jim Thompson wrote:
>> On Tue, 22 Mar 2011 15:42:36 -0700, Joerg <i...@invalid.invalid>
>> wrote:
>> 
>>> Jim Thompson wrote:
>>>> On Tue, 22 Mar 2011 10:51:26 -0700, Joerg <i...@invalid.invalid>
>>>> 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

Re: PSpice worst case simulation - Joerg - 2011-03-22 19:42:00

k...@att.bizzzzzzzzzzzz wrote:
> On Tue, 22 Mar 2011 13:31:11 -0700, Joerg <i...@invalid.invalid> wrote:
> 
>> Jim Thompson wrote:
>>> On Tue, 22 Mar 2011 12:54:35 -0700, Joerg <i...@invalid.invalid>
>>> wrote:
>>>
>>>> Jim Thompson wrote:
>>>>> On Tue, 22 Mar 2011 12:43:19 -0700, Joerg <i...@invalid.invalid>
>>>>> wrote:
>>>>>
>>>>>> Jim Thompson wrote:
>>>>>>> On Tue, 22 Mar 2011 11:58:51 -0700, Charlie E. <e...@ieee.org>
>>>>>>> wrote:
>>>>>>>
>>>>>>>> On Tue, 22 Mar 2011 10:49:21 -0700, Joerg <i...@invalid.invalid>
>>>>>>>> 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.

Re: PSpice worst case simulation - Joerg - 2011-03-22 19:52:00

Jim Thompson wrote:
> On Tue, 22 Mar 2011 16:23:59 -0700, Joerg <i...@invalid.invalid>
> wrote:
> 
>> Jim Thompson wrote:
>>> On Tue, 22 Mar 2011 15:42:36 -0700, Joerg <i...@invalid.invalid>
>>> wrote:
>>>
>>>> Jim Thompson wrote:
>>>>> On Tue, 22 Mar 2011 10:51:26 -0700, Joerg <i...@invalid.invalid>
>>>>> 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.

Re: PSpice worst case simulation - Joerg - 2011-03-23 21:20:00

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.

| 1 | 2 | | 4