AD8436 : MODEL SPICE (une fois de plus!!)

Hi,

I can't use AD8436 spice model  with pspice .

The output file contains :

X_U5.B3 +15V -15V X_U5.I X_U5.IF V ---------------$ ERROR -- Invalid parameter + IBUFVP -V VEE 4.8 160u 0

X_U5.B4 +15V -15V X_U5.I X_U5.IF V ---------------$ERROR -- Invalid parameter+ OBUFVP -V VEE 4.8 40u 0
X_U5.B5 +15V -15V X_U5.I X_U5.IF V----------------$ERROR -- Invalid parameter

I've changed the last line (.end change by .ends) and the line about B2 (B2 0 OUT I=I(V16) change by B2 0 OUT I=I{V16})

Could you tell me what is the right syntax for pspice ?

Thank you.

Parents
  • 0
    •  Super User 
    on Jul 8, 2019 4:49 PM over 1 year ago

    Hello,

    B-sources are defined in some SPICE-programs like LTspice, but PSPICE has another syntax for this kind of sources.

    You should replace the B-sources below with equivalent G-sources using VALUE=.'
    I have  done this for the  four B-sources in the model file AD8436.cir. Therefore I made the original SPICE-lines to comment with this character * in the first column and added the equivalent PSPICE-line in the next line. Please try with these changes.

     

    *B3 IBUFVP VEE I=IF( (V(IBUFVP)-V(VEE) ) > 4.8, 160u, 0)

    GB3 IBUFVP VEE VALUE = {IF( (V(IBUFVP)-V(VEE) ) > 4.8, 160u, 0)}

    *B4 OBUFVP VEE I=IF( (V(OBUFVP)-V(VEE) ) > 4.8, 40u, 0)

    GB4 OBUFVP VEE  VALUE = {IF( (V(OBUFVP)-V(VEE) ) > 4.8, 40u, 0)}

    *B5 VCC VEE I=IF( (V(VCC) - V(VEE) ) > 4.8, 325u, 0)

    GB5 VCC VEE VALUE = {IF( (V(VCC) - V(VEE) ) > 4.8, 325u, 0)}

    *B1 0 CAVG I=I(V11)**2/ABS(I(V16))

    GB1 0 CAVG VALUE = {I(V11)**2/ABS(I(V16))}

    Source of the SPICE-model file AD8436.cir : www.analog.com/.../ad8436.html

    Best regards,
    Helmut

  • +1
    •  Super User 
    on Jul 8, 2019 7:08 PM over 1 year ago in reply to helmuts

    Hello,

    I have attached an example schematic and symbol for the simulation with LTspiceVII.
    It's nearly the circuit of figure 40 from the datasheet.

    By the way the schematic in figure 40 in the datasheet has a missing GND connection or a 4.7uF capacitor connected to pin IGND.

    Helmut

    I just replaced the zip-file, because I found  a wrong ".end" in the model file. It has to be ".ends".

    5344.AD8436_test1.zip

  • +1
    •  Super User 
    on Jul 8, 2019 9:57 PM over 1 year ago in reply to helmuts

    Hello,

    There is one more line which has to be replaced when using this model with PSPICE.

    *B2 0 OUT I=I(V16)
    GB2 0 OUT VALUE = {I(V16)}

    Again all the mentioned changes in the model file ad8436.cir

    *B2 0 OUT I=I(V16)

    GB2 0 OUT VALUE = {I(V16)}

    *B3 IBUFVP VEE I=IF( (V(IBUFVP)-V(VEE) ) > 4.8, 160u, 0)

    GB3 IBUFVP VEE VALUE = {IF( (V(IBUFVP)-V(VEE) ) > 4.8, 160u, 0)}

    *B4 OBUFVP VEE I=IF( (V(OBUFVP)-V(VEE) ) > 4.8, 40u, 0)

    GB4 OBUFVP VEE  VALUE = {IF( (V(OBUFVP)-V(VEE) ) > 4.8, 40u, 0)}

    *B5 VCC VEE I=IF( (V(VCC) - V(VEE) ) > 4.8, 325u, 0)

    GB5 VCC VEE VALUE = {IF( (V(VCC) - V(VEE) ) > 4.8, 325u, 0)}

    *B1 0 CAVG I=I(V11)**2/ABS(I(V16))

    GB1 0 CAVG VALUE = {I(V11)**2/ABS(I(V16))}

    *.END

    .ENDS

    Helmut

  • Thank you very much helmuts.
    I had already had this problem some years ago 
    and an expert had given me a solution that I lost (désolé!).
    But your explanations about the syntax differences between
    Lt spice and Pspice are clear.
    I made the changes and there are no more problems. Again, thank you very much.
     
  • +1
    •  Super User 
    on Jul 9, 2019 8:51 AM over 1 year ago in reply to SLE CHANU481

    Hello SLE CHANU481,

    Thanks a lot for your feedback. I am happy that this PSPICE-model works for you.

    I have attached the modifed subcircuit of the AD8436 for PSPICE.


    By the way it will work with LTspiceXVII too, because LTspiceXVII accepts this PSPICE-syntax too.

    Helmut

    ad8436.zip

Reply Children
No Data