Home > Community > Forums > Hardware/Software Co-Development, Verification and Integration > Pspice Advanced : SMOKE. Different smoke limits per Model

Email

* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

 Pspice Advanced : SMOKE. Different smoke limits per Model 

Last post Sun, Apr 14 2013 9:41 PM by alokt. 7 replies.
Started by Dami 08 Apr 2013 06:10 AM. Topic has 7 replies and 1811 views
Page 1 of 1 (8 items)
Sort Posts:
  • Mon, Apr 8 2013 6:10 AM

    • Dami
    • Not Ranked
    • Joined on Mon, Apr 8 2013
    • Posts 4
    • Points 80
    Pspice Advanced : SMOKE. Different smoke limits per Model Reply

    Hi,

     I start with the smoke analysis and I do not manage to create 2 resitances with different properties.

    I am used to add Rbreakout resistors and to Edit the Pspice Model in order to give them different DEV (for example 1% and 10%) or TC1.

    Now I would like to perform a smoke analysis on my design? is it possible?

    The "part" VARIABLES in PSPICE_ELEM library defines all the smoke limits but there are the same for all the resistors....

    Thanks

    Dam 

     

    • Post Points: 20
  • Mon, Apr 8 2013 7:05 AM

    • oldmouldy
    • Top 10 Contributor
    • Joined on Tue, Jul 15 2008
    • Woking, Surrey
    • Posts 1,410
    • Points 24,070
    Re: Pspice Advanced : SMOKE. Different smoke limits per Model Reply

    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.

    • Post Points: 20
  • Tue, Apr 9 2013 3:11 AM

    • Dami
    • Not Ranked
    • Joined on Mon, Apr 8 2013
    • Posts 4
    • Points 80
    Re: Pspice Advanced : SMOKE. Different smoke limits per Model Reply

    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 

     

    • Post Points: 20
  • Thu, Apr 11 2013 5:19 AM

    • alokt
    • Top 25 Contributor
    • Joined on Thu, Aug 21 2008
    • Noida, Uttar Pradesh
    • Posts 241
    • Points 3,470
    Re: Pspice Advanced : SMOKE. Different smoke limits per Model Reply

    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?

    • Post Points: 20
  • Fri, Apr 12 2013 2:03 AM

    • Dami
    • Not Ranked
    • Joined on Mon, Apr 8 2013
    • Posts 4
    • Points 80
    Re: Pspice Advanced : SMOKE. Different smoke limits per Model Reply

    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 

    • Post Points: 20
  • Fri, Apr 12 2013 6:16 AM

    • alokt
    • Top 25 Contributor
    • Joined on Thu, Aug 21 2008
    • Noida, Uttar Pradesh
    • Posts 241
    • Points 3,470
    Re: Pspice Advanced : SMOKE. Different smoke limits per Model Reply

    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?

    • Post Points: 20
  • Fri, Apr 12 2013 7:13 AM

    • Dami
    • Not Ranked
    • Joined on Mon, Apr 8 2013
    • Posts 4
    • Points 80
    Re: Pspice Advanced : SMOKE. Different smoke limits per Model Reply

    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)

    • Post Points: 20
  • Sun, Apr 14 2013 9:41 PM

    • alokt
    • Top 25 Contributor
    • Joined on Thu, Aug 21 2008
    • Noida, Uttar Pradesh
    • Posts 241
    • Points 3,470
    Re: Pspice Advanced : SMOKE. Different smoke limits per Model Reply

    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.

    • Post Points: 5
Page 1 of 1 (8 items)
Sort Posts:
Started by Dami at 08 Apr 2013 06:10 AM. Topic has 7 replies.