Help with PSpice Error

Yes:-)

Have a go with SuperSpice

The other reason is that there is a full set of tube/value symbols, and as a guitarist and analogue engineer as well, I know quite a bit about them e.g.

Kevin Aylward snipped-for-privacy@anasoft.co.uk

Joe, The first error is the Probe window saying that the data file generated is empty, i.e. there was no data to view. The second error of data overflow I am not familiar with! Sounds like the model is doing something that goes to infinity, either a super-high or current or voltage, or something else illegal. Would need to see both to be sure.

Charlie,

Experienced that myself recently, with PolarFAB BP30 NPN models that are subcircuits that include the parasitic PNPs to substrate.

Cured it by setting SOLVER=0 ;-)

...Jim Thompson

Thanks a lot for the replies! I was able to find out that the models were originally written for Intusoft PSpice 5.0. I'm using them with Orcad PSpice 10, and it was suggested that perhaps the command syntax is different.

The only real difference between this model and the one that works is the use of the POLY statement - which I'm finding to be rather confusing. Here are a couple of those statements:

eG0 10 0 poly(1) -3.7694e+00 1.9947e+00 5.9432e-02 eG1 11 0 poly(1) -3.2024e-02 -4.1443e-02 -4.8236e-03 eG2 12 0 poly(1) 1.9127e-02 -1.2189e-02 -1.5526e-03 eG3 13 0 poly(1) -1.1354e-02 4.9339e-03 6.1016e-04

eP0 110 0 poly(1) -9.9158e+0 1.9145e+0 -2.8135e+0 1.8661e+0

• 1.5643e+0 4.7240e-1 6.4276e-2 3.3101e-3

eP1 111 0 poly(1) 9.5428e-1 3.2558e-2 -8.3349e-1 -4.8578e-2

• 2.6213e-1 1.0492e-1 1.8921e-2 1.3632e-3

eP2 112 0 poly(1) 9.5766e-2 2.5192e-2 2.2391e-1 -1.7040e-1

• -2.4952e-1 -1.0960e-1 -2.0981e-2 -1.4882e-3

eP3 113 0 poly(1) -6.6107e-2 -3.9657e-2 7.5560e-2 3.1025e-2

• 2.4265e-2 1.7002e-2 4.2512e-3 3.4761e-4

eP4 114 0 poly(1) 8.4148e-3 4.7989e-3 -1.3258e-2 -1.9288e-3

• 5.2888e-4 -5.6853e-4 -2.4727e-4 -2.4359e-5

I can't tell if there are any glaring syntax problems or not, but from the reading I've don, I think these lines are okay for use with Orcad.

Joe, Looks like the problem is the instead of regular (). All the PSpice examples I have show ().

You finally worked your own way thru the problem and made it easy for me to appear wise ;-)

Bound v(1,3) so that it can't be ZERO (or fudge the operand so it can never be ZERO).

...Jim Thompson

Thanks Charles. I just tried changing the characters to ( ), and I see the same error. Specifically, this error occurs when calculating the bias point for the transient analysis. In the output file is:

INTERNAL ERROR -- Overflow, Convert

I did find the following excerpt from the PSpice manual regarding the POLY statement which seems to apply to this problem, though I'm not quite sure:

" Caution must be exercised with the POLY form. For instance,

EWRONG 1 0 POLY(1) (1,0) .5 1.0

tries to set node 1 to .5 volts greater than node 1. In this case, any analyses which you specify will fail to calculate a result. In particular, PSpice A/D cannot calculate the bias point for a circuit containing EWRONG. This also applies to the VALUE form of EWRONG: (EWRONG 1 0 VALUE = {0.5 * V(1)}). "

I took a closer look at the PSpice manual section below, and realized it related to the VALUE statement also - which does exist once in this model as follows:

eGIogVpc 20 0 value={log(v(1,3))}

I tried rephrasing this as

eGIogVpc 20 0 value={1}

and the simulation error disappeared! The results are entirely inaccurate, but I think this confirms that the problem is with VALUE and not POLY.

Now it's just a matter of figuring out why... :-)

What Jim Said! 8-)