Electronic – LTSpice current dependent current source timestep too small error

circuit analysisltspice

I solved this circuit by hand.Which asks to calculate vo and Io in the circuit.

Transistor circuit

And I tried to verify results with LTSpice.

LTSpice circuit

If I change dependent current source B2's equation to I = I(R1)* 50 it gives an error like that:

LTSpice error

If I use I = I (R1) it works fine. What might be the problem here?

Best Answer

If you open up the manual (F1) and look at LTspice > Circuit Elements > B. Arbitrary Behavioural Voltage or Current Source, you'll see this bullet point:

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.

What you have there is a direct feedback which violates the above condition. If, instead of behavioural sources, you use primites such as VCVS and CCCS, everything works:


For the CCCS, I have used V1, for comodity, since it's already there, otherwise you would have had to add a zero-valued voltage source in series with R1 (with correct polarity).

As a side note, in your schematic, you're labeling the ground net with C, which can be done, but it's completely useless. IIRC, except the ground, naming the same net more than once means LTspice will use the latest label.

Also see this answer, it's the same.