[Lowfer] Re: PSpice simulation

[James Moritz]

Dear Bill, Lowfers,

At 04:01 30/08/2002 -0400, you wrote:
>Another discovery I made was that this version has a coax cable model
>(listed as 'T' in the library) but I can't seem to get it to work, even with
>the simplest of circuits. There are TD, F, and NL attributes required, as
>well as the Zo, but the simulation chokes no mater what values I put in. Has
>anyone used this function?

TD = line delay (s)
NL = number of electrical wavelengths (if no value entered defaults to 0.25)
F = frequency at which number of wavelengths is specified (Hz)

You should specify EITHER NL and F, OR TD, but not both - obviously a 
conflict will arise in that you are effectively specifying the same thing 
in two different ways, if you specify both the electrical length and the 
propagation delay.

There is also "TLossy", a lossy transmission line model where you specify 
the length and R,L,G,C, distributed line parameters, and various other 
lumped transmission line models - refer to a transmission line text book 
for further explanation!

Always bear in mind that you have to give the simulator accurate 
information to stand any chance of getting a sensible result - this means 
you must include things like stray inductance, capacitance and resistance 
if these have a significant effect on the operation of the circuit, as they 
usually do in a PA for example. If the simulator thinks that a piece of 
wire has 0 resistance, it is only reasonable that an infinite current will 
flow in it if a voltage is applied... this means that if you use "perfect" 
inductors and capacitors in a filter, with a lossless transmission line, 
there will be frequencies at which the impedances are zero and infinity, 
with consequent infinite voltages and currents, or at least as near 
infinity and zero as the computer can get when overflows occur. This does 
not always cause the simulation to crash, so scrutinise the results 
carefully, and if in doubt consult an oscilloscope!

Cheers, Jim Moritz
73 de M0BMU