SPICE capacitance question

[Tim Williams]

Is there any such thing as a box you can put on a node to measure its
capacitance? XSPICE (or some variants thereof) at least comes with a
"CMETER" entity, but it only appears to measure passives, not dynamic
(semiconductor junction or synthesized) capacitances. How useless.

There's always the old charge-it-with-a-waveform (usually CCS to make a
voltage ramp, or voltage ramp to make current), then C = I / (dV/dt), but
that obviously doesn't work if there's bias or leakage current.

Tim

 

[Jamie]

Is there any such thing as a box you can put on a node to measure its
capacitance? XSPICE (or some variants thereof) at least comes with a
"CMETER" entity, but it only appears to measure passives, not dynamic
(semiconductor junction or synthesized) capacitances. How useless.

There's always the old charge-it-with-a-waveform (usually CCS to make a
voltage ramp, or voltage ramp to make current), then C = I / (dV/dt), but
that obviously doesn't work if there's bias or leakage current.

Tim

I've been hashing a little with LTspice lately with making a model or
sort of for an SCR.

I've succeeded in making a sub circuit connectable in a block using the
primitive functions of spice, current sources, voltages sources etc..
but would like to get a better understanding of the model code itself.

It seems that finding the resources needed for the actual event
variables that you need to access in your model code and label variables
for C, R, L on inputs and outputs etc are hard to locate..

I do programming in various languages so I have a good idea on how
this should all work. I have looked at various models already and have
gotten many of my questions answered how ever, It would be nice if there
was a plain document on the step by step of the primitive variables that
are involved and the names of them you need to know in the model code.

Set sizes , cycle count and things of that sort, so that one can
quickly put together a working step circuit.. if you get my drift.

The help file, as good as it is, offers you all the math functions and
the like but it seems to come in short when it wants you to understand
the under layer of what is to be taken place.

For example, I saw in one example the use of ro, lo, co, ri, ci, li to
indicate the basic elements R,L,C in the input or output which makes
perfect sense how ever, If that is to be primitive variables of spice, I
can't find that documented? Or, what I saw isn't what it is.

Years ago in college I didn't use anything like spice, we did it all
on paper and slide rules. Then I got my first TI si calculator and that
was a big jump for me

Jamie

 

[Tim Williams]

How about pumping in a sine wave current source and amplifying the
node voltage into a synchronous detector and lowpass filter? Or maybe
just FFT it.

AC analysis is the obvious solution, but you have to set the DC operating
point. Each. And. Every. Time. Remember, I said it's a variable
capacitance. Sure, you can set a parameter sweep with the bias, but then
you get, say, a hundred curves with >2 points per curve and no curve
connecting the curves.

Tim

 

[Tim Williams]

This sounds useful, unfortunately it would have to be implemented in a
scripting language (DelphiScript, JS, etc.) working with Altium's API, if
it even provides handles to automate this sort of thing in the simulation
editor.

Tim

 

[Tim Williams]

Why not design a c-meter and run it in time-domain mode? Just probe
its output like any other signal.

Supposing I run bias from a staircase source (creating the transient
equivalent of the AC + parameter sweep setup), I have to wait for ALL
signals to stabilize, both bias AND the c-meter reading. This will take
more than a few cycles of whatever the c-meter is doing, and a hundred
points will take several minutes to simulate.

Then if I want to incrementally tweak the model I'm testing, I have to
wait several minutes again.

Plus the time of designing and building the setup in the first place,
which is probably a few hours, depending on how involved the c-meter is
made to be. It doesn't have to be fancy since it could be e.g. current
sources, switches, charge pumping, that sort of thing, but those all cost
simulation time.

Tim

 

[legg]

Is there any such thing as a box you can put on a node to measure its
capacitance? XSPICE (or some variants thereof) at least comes with a
"CMETER" entity, but it only appears to measure passives, not dynamic
(semiconductor junction or synthesized) capacitances. How useless.

Semiconductor junction capacitances are currently characterized base
on curve fiting of static data, and the characteritics are applied
dynamically. Are you suggesting that this does not reflect real
situations?

There's always the old charge-it-with-a-waveform (usually CCS to make a
voltage ramp, or voltage ramp to make current), then C = I / (dV/dt), but
that obviously doesn't work if there's bias or leakage current.

Tim

As in real life, you'd have to couple the 'tester' to the node in
question, to minimize loading effects or interference in function. The
issue isn't avoided, just because it's a simulation.

Complex impedance measurements can be made, conventionally, to extract
reactive components.

It's a little ironic, as the solution to any spice node's
characteristics should be solvable mathematically - it is a construct,
after all. As we adopt models and tools that are more complex - that
we don't completely understand - we require more complex test features
to 'simplify' the process of understanding.

I wonder if, in the end, we know more, or less?

Constructing the spice equivalent of test equipment is an activity
that is being tried from a number of directions in the LTspice yahoo
group. This has included curve tracers and impedance/network
analysers.

RL

 

[Tim Williams]

As in real life, you'd have to couple the 'tester' to the node in
question, to minimize loading effects or interference in function. The
issue isn't avoided, just because it's a simulation.

Complex impedance measurements can be made, conventionally, to extract
reactive components.

That's all fine and dandy, but like I said to John, if I implement it
conventionally, I have to wait for it to stabilize. I'd love to do it in
real time, because heck, I can generate that fast enough to sweep a CRT
scope, let alone generate some X-Y points on the DSO in under a second.
But doing it in sim is a lot more painstaking. I was hoping someone might
have an elegant solution which takes advantage of the environment.

Tim

 

[legg]

Do a .AC analysis, with the excitation named (reference designator)
"VAC". Then...

CAPINT=IMAG(-I(VAC))*IMAG(-I(VAC))-REAL(-I(VAC))*REAL(-I(VAC))
CAPRES=REAL(-I(VAC))/CAPINT
CAPVAL=CAPINT/IMAG(-I(VAC))/(2*pi*FREQUENCY)

If you want capacitance versus bias, parameterize the bias, run the
.AC, then use Performance Analysis to plot capacitance versus bias.

(This is in PSpice, but I'm sure a comparable method exists in
LTspice.)

...Jim Thompson

If only Tim would read postings to the bottom of the page, he might
get somewhere, intead of stewing.

There are all sorts of ways to reduce simulation time. Establishing
initial operating conditions is only one of them, though in my line of
work it would avoid useful hints about relevant disasters-in-waiting.

RL