Pspice Advanced : SMOKE. Different smoke limits per Model

DEV is a Tolerance parameter for use with Monte Carlo or Worst Case Analysis and the TC parameters are for the SPICE related coefficients for Value variations with Temperature. You need to look at the MAX_TEMP, POWER, SLOPE parameters for resistor stress parameters, you can override these for each component, rather than use the "Variables" values. The PSpice Advanced Analysis User Guide, pspaugca.pdf in the doc\pspaugca directory of the installation covers Advanced Analysis, Smoke and the "for Power Users" section covers the parameters and what they mean to the analysis.

BTW: you can add as many user defined Variables as you need so you could have multiple definitions for RMAX, like RMAX1, RMAX2 and so on, give these a value in "Variables" and then change the RMAX property value on the component(s) to apply them.

Thank you oldmouldy!

 Ok I managed to create several (RMAX1, RMAX2,..) and by giving them different "SIZE" (SIZE1, SIZE2,...) it appears as different parts in my Bill of Materials (BOM)!

Now I'm trying to perform a Monte Carlo.
I have a SUBCKT with inside this model:
.MODEL RMODEL RES ( R=1 DEV={0.0005*DEVTOL+10e-6*DTEMP+15e-6*DMONTH} )
In my design I have declared 3 parameters named DEVTOL, DTEMP, DMONTH.
And it was working well.

Now I have add around this SUBCKT resistor from pspice_elem.
And when I select "Enable PSpice AA support for legacy", it seems that Pspice does not evaluate the { } expression anymore.
When the 3 parameters are set to 0, I still have a DEV=0.0005.

Is it a know problem?

Thanks 

Resistor from PSpice_ELEM would have it's own model & hence tolerance parameter/calculation. Are you saying you have modified the RESISTOR form PSpice_elem library to have model defined as ( R=1 DEV={0.0005*DEVTOL+10e-6*DTEMP+15e-6*DMONTH} )

How?

Also when you say "... PSpice does not evaluate the { } expression anymore",  can you explain how did you arrive at this conclusion? Are you concluding this based on results shown in PSpice Advance Analysis or PSpice?

No I did not change the Resistor from PSpice_ELEM.

I have a schematic with several AD587U, op97, and resitors. 

I have modified the AD587U/AD in order to have Monte Carmo analysis in Pspice.
I create the RMODEL above to have a model conform to the datasheet i.e. 10V+/-5mV.

I didn't realize that PSpice Advance Analysis and Pspice A/D were 2 separate software.
I just notice that when I select "Enable PSpice AA support for legacy", then the PSpice A/D result are wrong.

I perform a Monte Carlo with  DEVTOL=0, DTEMP=0, DMONTH=0, PSpice A/D show me a histogram with the output always equal to 10.0V.

I perform a Monte Carlo with  DEVTOL=1, DTEMP=10, DMONTH=60, PSpice A/D show me a histogram with the output which vary between [9.982 and 10.018]. That's Ok.

I perform a Monte Carlo and i select "Enable PSpice AA support for legacy" with  DEVTOL=0, DTEMP=0, DMONTH=0, PSpice A/D show me a histogram with the output which vary between [9.995 and 10.005]. That's Wrong.

Thanks to your help, I now manage to have a SMOKE analysis.
In the Pspice Advanced Analysis Interface, I am not interested in some parameters (for example "Maximum current" for a capacitor) but some other parameters (like the "Maximum temperature" for a capacitor) are not visible.
Is it possible to choose?

I just hide the "Max current" by filtering but I do not have the Max Tem on capacitors and I have it on the resistors??

And is it possible to extract the results to present them in another report ( something like a Copy to clipboard?)
Because the interface with green histogram it really intuitive!

Thank you 

Capacitor "C" is ideal component and hence you do not see any temperature parameter, as there will not be any power loss. C_t component from analog.olb, should have temperature parameter as this is modeled with ESR (for smoke analysis only, in simulation it is still ideal C)

About report:  No, in current version you do not have ability to copy results (BAR etc ). If you copy paste, if would paste just grid data, with some additional details, but not the green/yellow/red bars. Screen capture is only alternate. You may want to file a service request for same.

Will check on "... i select "Enable PSpice AA support for legacy" with DEVTOL=0, DTEMP=0, DMONTH=0, PSpice A/D show me a histogram with the output which vary between [9.995 and 10.005]. That's Wrong."

Which release version of PSpice you are currently using?

Thank you for the details about the capacitor now I understand.
The "C" capacitor from PSpice_ELEM has a property MAX_TEMP and the VARIABLES has a poperty CMAX.
They are used for what purpose?

My versions :
OrCAD Capture 16.6-p005 (v16-6-112D)
 PSpice 16.6p003 (v16.6-112B)

CMAX property in variable block is generic property placeholder and value assigned to CMAX under variables, would be substituted for Maximum Rated Voltage on all capacitors.

Capacitor part from PSpice_ELEM library would also show temperature derating of it's max rated voltage due to ambient temperature (simulation temperature). This derating is modeled using MAX_TEMP, KNEE ,SLOPE parameter.

Hope this clarifies.