• State Resolved
  • Locked Locked
  • Replies 2 replies
  • Subscribers 37 subscribers
  • Views 783 views
  • Users 0 members are here
Support feedback
Options
Options
Related

This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

OPA320/OPA320S Model doesn't work in PSPICE v8.0

George Barbehenn
Prodigy 100 points
Other Parts Discussed in Thread: OPA320

The OPA320/OPA320S PSPICE model doesn't work, at least in version 8.0 of PSPICE.

The capacitors in the root subcircuit have a TC ("TC=0,0") which the simulator doesn't recognize.  Since the coefficients are 0, it isn't needed, in any event.

The E and G devices have all 4 terminals defined and an evaluate ({...}) for the gain.  The simulator does not support an evaluate for E and G devices with all 4 terminals defined.  The control terminals should be moved in the evaluate term:

Ey 1 2 3 4 {gain}  ==> Ey 1 2 {V(3,4) * gain}

or

Gy 1 2 3 4 {gain} ==> Gy 1 2 {V(3,4) * gain}

ghb

  • 0
    TI__Mastermind 41310 points

    George,

    PSpice does support TC's for resistors and capacitors, however, in this case, since they are all set to 0, I would simply remove them. Are you using PSpice 8.0 or a simulator based on PSpice 8.0?

    PSpice does support this context for E/G sources. Please refer to the PSpice manual:

    General form E<name> <(+) node> <(-) node> <(+) controlling node> <(-) controlling node> <gain>

    E<name> <(+) node> <(-) node> POLY(<value>)

    + < <(+) controlling node> <(-) controlling node> >*

    + < <polynomial coefficient value> >*

    E<name> <(+) <node> <(-) node> VALUE = { <expression> }

    E<name> <(+) <node> <(-) node> TABLE { <expression> } =

    + < <input value>,<output value> >*

    E<name> <(+) node> <(-) node> LAPLACE { <expression> } =

    + { <transform> }

    E<name> <(+) node> <(-) node> FREQ { <expression> } = [KEYWORD]

    + < <frequency value>,<magnitude value>,<phase value> >*

    + [DELAY = <delay value>]

    E<name> <(+) node> <(-) node> CHEBYSHEV { <expression> } =

    + <[LP] [HP] [BP] [BR]>,<cutoff frequencies>*,<attenuation>*

     

    Examples

    EBUFF 1 2 10 11 1.0

    EAMP 13 0 POLY(1) 26 0 0 500

    ENONLIN 100 101 POLY(2) 3 0 4 0 0.0 13.6 0.2 0.005

    ESQROOT 5 0 VALUE = {5V*SQRT(V(3,2))}

    ET2 2 0 TABLE {V(ANODE,CATHODE)} = (0,0) (30,1)

    ERC 5 0 LAPLACE {V(10)} = {1/(1+.001*s)}

    ELOWPASS 5 0 FREQ {V(10)}=(0,0,0)(5kHz, 0,0)(6kHz -60, 0) DELAY=3.2ms

    ELOWPASS 5 0 CHEBYSHEV {V(10)} = LP 800 1.2K .1dB 50dB

    GBUFF 1 2 10 11 1.0

    GAMP 13 0 POLY(1) 26 0 0 500

    GNONLIN 100 101 POLY(2) 3 0 4 0 0.0 13.6 0.2 0.005

    GPSK 11 6 VALUE = {5MA*SIN(6.28*10kHz*TIME+V(3))}

    GT ANODE CATHODE VALUE = {200E-6*PWR(V(1)*V(2),1.5)}

    GLOSSY 5 0 LAPLACE {V(10)} = {exp(-sqrt(C*s*(R+L*s)))}

    I am unsure of  all of the limitations of PSpice V8.0, but if it is a free version of PSpice there are several limitations and this may be one of them as well as the node limits that will surely apply.

    The current version of PSpice is version 17.2.

  • 0 in reply to Britt Brooks - Online Design Tools
    Prodigy 100 points
    Britt:
    I have two copies of the *full* Design Center 8.0, as I used to be a beta site for PSPICE. Besides the fact that I own these, they aren't rentware, so they don't 'expire'. These are not eval or student versions, but the complete versions with PLSyn, PCBoards, Optimizer, Polaris, etc.

    PSPICE does *not* support TC for capacitors, at least in version 8.0. Models should be backward compatible, so if TC was added to capacitors sometime before 17.2, including TC in the models will break the netlist readin.

    I was stating what you listed from the manual, ut supra. The distribution OPA320/OPA320S model from TI, *uses the 4 node notation and includes an evaluate ({...}) for the gain.* This is *not* supported as you documented. Therefore to fix the problem it is necessary to change those lines as I showed ut supra.

    After I make these changes to the models, they work fine and I can simulate my 4 quadrant current sense just fine. However, the above 'errors' in the models appear to me to be the outcome of a netlister error? Whatever tool you are using to produce the model subcircuit netlist from (I presume) a schematic, is hosing the model. So, it would be better to fix the netlister, which is why I mentioned it.

    Finally, if you want a model that allows a capacitor to have a TC that is backward compatible with PSPICE versions 6.1 ~ now, please let me know. It also provides a tabular dependence of capacitance on DC bias, if you'd like.