OPA2863A: PSPICE model has duplicate(?) noise and bias current entries.

Hi Renan,

Thank you for sharing this information. Some of the duplicate components you mentioned were put in place to simulate this specific device which is why it appears different than the other models we usually release. We will look into this model and the suggestions you have made.

Best Regards,

Ignacio

Hello Ignacio,

 If it is correct, it is correct, it just seemed odd to me.

    The only further thoughts I have:

1) It seems like the "-" input noise sources (X_I_NN         ESDN MID, X_I_NN1         ESDN MID , and R184&amplifier/filter)  could be combined into one X_I_NN, as they are in parallel?  Actually, X_I_NN and X_I_NN1 are redundant, full stop, as you could have one subcircuit with different parameters, that subsumes both.

2) It seems like the "+" input noise sources (X_I_NP, and R182 and R183 amplifier/filters) could be subsumed into X_I_NP, as they are in parallel?

This would reduce the clutter, make the model much easier to maintain, and make the functionality evident.  That is what I'm going to do.

Also, the generic comments still apply:

1) Older PSPICE versions (i.e. 8.0, 9.2) and other versions of SPICE don't support the "TC=0,0" syntax for resistors, and the default is TC1=0, TC2=0 anyway.  Don't have a value for these schematic symbol attributes, and netlist with the "?", in the template, so that they netlist *properly* when there is a value other than the default.

2) Older PSPICE versions (ditto) and other versions of SPICE don't support "+" and "-" in *.subckt node names*.  You should be using "plus" and "minus".

I've attached the OPAx863 (TI only has the model on the OPA2863 product page, and the model is called "OPA2863", with the changes to the noise generation we discussed.  I'm still doing the various sources with tolerances, but you can see how moving the noise generation into the V, I+, I- noise subcircuits makes the model easier to understand, use and maintain.

    I very much think that the two current noise sources, with both use FEMT, could be subsumed into one subcircuit.

OPAx863A working model.zip

Regards,

Renan

Hello Ignacio,

Any update?

Regards,

Renan

Hi Renan,

We adjust the models to work with TI for PSpice as well as TINA-TI, however they also work in other spice simulators. Are you seeing a problem with the model in your simulator?

Best Regards,

Ignacio

Hello Ignacio,

Please see the response from the customer below:

I first used PSPICE in 1987 (yes, in DOS), as was a beta site for PSPICE for 6 years.  Although I have a copy of PSPICE for TI, latest version, I also own copies of PSPICE 8.0 from my days as a beta site.

    The syntax "TC=0,0" for the quadratic temperature coefficients of a resistor is very recent in PSPICE, if at all.  And, as I said, is redundant, as the default is TC1=0 and TC2=0.  Are you using TINA with Capture?  Probably not, so just change the TEMPLATE in the Capture GWL model schematic to netlist the resistors properly.  The use of "+" and "-" in *subcircuit node names* is also a very recent development, if at all.  So, again just name the subcircuit nodes with "plus", instead of "+", and "minus", instead of "-".

    Finally, TI often ships E(or G) VALUE netlisted as (from the OPA2863 model):

E1 3 6 7 8 {GLFF}

    when the correct syntax is:

E1 3 6 Value={V(7,8)*{GLFF}}

    I can also share with you a "new and improved" GWL model, as the current TI GWL model has some serious issues.  Most notably, the currents being summed at the CLAW_CLAMP node are out of phase with one another, and this problem is insoluble in the current topology.  Let me know if you want the new topology I've come up with, as it seems to work.

Regards,

Renan