[SOLVED] LTSpice IV simulation problem.

The following circuit (stability measurement) shows a problem: The simulation waits to show curves forever (well, I did not wait that long), and when I interrupt the simulation manually it shows the error "Failed to find the DC operating point for AC analysis".


When I however connect Vfb (feedback voltage) to the connection of R1 and R2 in stead of to the voltage source B2, the simulation works fine, as shown in the curves above. (the curves are from the "simulatable" version of the diagram).

I've tried changing almost all parameters in the LTSpice IV control panel (including checking "NoOpiter"), but nothing helps.

Anyone any idea? Thanks in advance!

The files:
I've also added the log file in case it reveals the reason for the problem.

Sometimes it helps the simulation, if you install a low-ohm resistor inline with a component. Example, the leg containing L3 has a supply but no resistance, therefore it cannot calculate an L/R time constant. Elsewhere the circuit has plenty of resistors, so the problem may be elsewhere, I don't know.

Also, you have L1 bypassed with a wire. This is not a fault with hardware, but the simulator may not know what to make of it. It may create an unrealistically long time constant. Anyway it's worth a try to see if the problem is reduced by putting a low-ohm resistor inline with L1.

BradtheRad said:

Sometimes it helps the simulation, if you install a low-ohm resistor inline with a component. Example, the leg containing L3 has a supply but no resistance, therefore it cannot calculate an L/R time constant. Elsewhere the circuit has plenty of resistors, so the problem may be elsewhere, I don't know.

Also, you have L1 bypassed with a wire. This is not a fault with hardware, but the simulator may not know what to make of it. It may create an unrealistically long time constant. Anyway it's worth a try to see if the problem is reduced by putting a low-ohm resistor inline with L1.

Click to expand...

Hi Brad, thanks for your reply. No success however, adding a series resiststor to L3 does not solve the problem, and also removing L1 is not.
I can make the simulation "start" again by making RLoad 5 ohms, but the results have no meaning: the gain is always (at any frequency) -390dB and the pase always -180 degress.
Any other ideas? Thanks in advance!

Review the LTspice help for behavioral sources to know why V=I(RLoad)/10 doesn't work:

Expressions can contain the following:

o Node voltages, e.g., V(n001)

o Node voltage differences, e.g., V(n001, n002)

o Circuit element currents; for example, I(S1), the current through switch S1 or Ib(Q1), the base current of Q1. However, it is assumed that the circuit element current is varying quasi-statically, that is, there is no instantaneous feedback between the current through the referenced device and the behavioral source output. Similarly, any ac component of such a device current is assumed to be zero in a small signal linear .AC analysis.

Click to expand...

I agree this behavior isn't expectable at first sight. Could use this circuit:

Hi FvM, thanks very much.

That did the trick!. I should better read the manual... Curiously the same construction (the one with the V=I(RLoad)) worked well in the transient analysis...