开云体育

I've never tried it with a switcher, but once I looked at the ripple voltage and current at the reservoir capacitor of a simple power supply, and saw what appeared to be a 'ghost' of the series inductor (limiting inrush current) on the AC side affecting the phase angle. Changing the inductor value changed the phase a bit. This 'ghost' inductance might series resonate with the lossless capacitor so as to produce oscillations. Could be worth investigating.

For resevoir and pump capacitors in switchers, I have found that adding ESR close to reality for the capacitor type, size and capacitance makes things better.

I have also found that adding some milliohms to model trace resistance in to and out of switchers helps.

开云体育

Yes, I tried. All I get are selections on GD and phase.

Only for Bode. If you choose the Cartesian format, you can get imaginary. what other options do you want?

?

For example, in using the s parameter script it would be nice to plot transmission gain s21 and SWR (for which I have a simple

expression) on left and right axis of a single plot pane. Are there more plot options if I rev up from LTspice XVII?

S-parameters of 1 and 2 port networks are automatically available as plot options if you use the .NET directive with .AC analyses. This then gives you the options: Sxx, Yxx, Zxx, Zin & Zout.

See: Help > LTspice > LTspice? > Dot Commands > .NET — Compute Network Parameters in a .AC Analysis

For SWR and other formats like Gmax and MSG, I have defined plot functions, which are stored in the plot.defs file. Hardly anyone actually uses plot.defs, but it's very useful once you get used to it.

E.g.:

* Functions for RF design using S-parameters with 2 port networks
* Note: due to the way LTspice displays functions (as voltages), MSG & Gmax are exported as square roots since they are powers to start with
.func mS11() {mag(S11(V1))}
.func mS21() {mag(S21(V1))}
.func mS12() {mag(S12(V1))}
.func mS22() {mag(S22(V1))}
.func DeltaInt() {S11(V1)*S22(V1)-S12(V1)*S21(V1)}
.func MSGInt() {ms21()/ms12()}
.func KR() {(1-ms11()**2-ms22()**2+mag(DeltaInt())**2)/2/mag(S21(V1)*S12(V1))}
.func GmaxInt() {1/(Kr()+sqrt(Kr()**2-1))*MSGInt()}
.func MSG() {sqrt(MSGInt())}
.func Gmax() {sqrt(GmaxInt())}
.func VSWR(Sxx) {(1+mag(Sxx))/(1-mag(Sxx))}

(Functions including "Int" are not for plotting, they are intermediate functions.

Note: if you edit plot.defs (Plot Settings > Edit Plot Defs file), the changes don't become active until LTspice is closed and re-started.

--
Regards,
Tony

开云体育

Right side of plot window is assigned to phase.?

?

Anyway to "hack" and assign right side of plot window?

to another parameter??

(This only applies to plots in the frequency domain.)

Did you try to change it?

If you bring the cursor close to the left axis, its appearance will change to a ruler. You can right-click and you will get a dialogue where you can change the quantities plotted: Bode, Nyquist or Cartesian.

For Bode, you can choose either phase or group delay, or none, by right-clicking on the right axis.

--
Regards,
Tony

开云体育

What I'm trying to determine is inrush current, so I have a PWL voltage source set to mirror what the external power supply will do when the test is performed for real. I happened to have it going from 0 volts at 1 ms to 28 V at 2 ms (because the test is defined in ms, and I like to steer clear of whatever SPICE does at time 0). Sometimes it's good to leave a problem overnight, and in the middle of the night I realised the model always fell apart before it got to 1 ms.? ?So this morning I simply changed the voltage generator to go from 0 at 1 ?s to 28 V at 1 ms, and the problem went away >doh!<. I do still need the .OPTIONS line above, but I'm using the default integration method (which is trapezoidal on LTSpice 24).

?

So there's another way to address the problem; timeshift the model so the circuit is doing something different at the time when the non-convergence kicks off.

While changing the time base in some way can apparently cure the #Time-step-too-small problem, it can also do the reverse, as can any other circuit change. You also don't mention whether you have set a maximum time step. Sometimes this also makes the issue disappear.

The underlying issue remains that one or more of the models is dodgy in some way.

--
Regards,
Tony