RST Engineering (jw) wrote:
Agreed, John, 150 MHz is damned near DC for a lot of us, but as yet I have
no answer from the "spice" folks for the 1 nf capacitor question. A lot of
fancydancing but no answers.

Jim

I didn't realize that this question was addressed to all "'spice'
folks", but was directed only to the OP. That's probably why the
"'spice' folks" haven't leapt to respond. Anyone who uses SPICE
professionally, and indeed a great number of amateur users should be
able to answer the question easily.

At 150 MHz, a capacitor lead can generally be handled as a single lumped
inductance. The amount depends on the wire's diameter and environment,
but around 7 nH is a good working number for a half inch lead. The
inductance of the capacitor body itself might have to be included in the
model if high accuracy is important. Capacitance to ground, from both
the leads and the capacitor body, might also be important if the
impedance of the circuit to ground is high. If so, it can be included.
The way I'd approach inclusion of the C would be to calculate the
impedance and length of the transmission line comprised of the lead and
ground plane or capacitor body and ground plane, then convert those
values to a single series L and shunt C rather than just directly using
a transmission line model -- very short transmission lines in a model
can greatly slow SPICE calculations unless there are also other very
short time constants involved.

On the other hand, if the "leads" are PC traces over a ground plane,
shunt capacitance will be higher, and the approach I mentioned with the
transmission line is the way I'd always do it. The model for the leads
would include both L and C. As an example, if the "lead" is a .010"
trace on .032" FR4 material (er ~ 5) over a ground plane, it makes a
transmission line of Z0 = 105 ohms, velocity factor 0.55. The equivalent
L and C of a half inch of this line are 8 nH and 0.73 pF respectively.

Other characteristics of the capacitor such as ESR might have to be
included in the model depending on the application.

You gave a capacitor value in your question -- an ideal capacitor of
that value would of course be the other part of the model.

SPICE is used daily, as it has been for decades, by professionals and
produces strikingly good results in the hands of someone who is skilled
at modeling and has a good understanding of the circuitry being modeled.
I've personally used SPICE for modeling linear to highly nonlinear
circuits up to 50 GHz, where even tiny SMT components were often modeled
as transmission lines and every pad and solder blob is significant and
included. The results were used in the design of products which have
been successfully produced by the thousands and sold for years.

Roy Lewallen, W7EL