LTspice third party model gives problem with transient analsys

Question

I have tried to import a third party model from TI, to be precise the op-amp A551. And somehow my circuite, a power amplifier, gives me the following error.

Analysis: Time step too small; time = 3.1653e-08, timestep = 1.25e-19: trouble with u2:jc-instance j:u2:4

It seems like my transient analsys is trying to hit a level of precision it just cant handle. The thirt party model was probably implemented correctly (I could be wrong), but why than doesnt the transient analsys work.

Answer 1

I see 3 mistakes you should correct before complaining about the op-amp model:

1. Reverse the emitter of the BDX54C PNP.
2. U2 is wired up as a non-inverting amplifier. This amplifier can provide a well-defined output voltage provided that it can drive the load. However, Q1 and Q2 with its resistor are wired as a transimpedance without much loop gain. They way you've wired it makes no sense. You probably meant to wire it @csabahu did it. The darlington stages provides drive capability to the amplifier and both of them must be within the feedback loop.
3. most importantly, your op-amp doesn't have any net supply voltages, as V2 is effectively +15V with respect to ground. Remove that (-) sign from the "-15" value of V2 or flip V2 such that the (+) sign is looking downwards. Your op-amp is right now, therefore, receiving +15V in both positive and negative supply pins.

Answer 2

Try fixing this first: -

Also note that some models are a bit flakey and sometimes you have to change the calculation engine or precision settings.

Answer 3

The factory model of the amplifier works fine. You have both transistors identical (BDX54C), this is probably a mistake. The wiring of the lower transistor is also faulty. I think you wanted to do something similar to the schematic below: In the schematic, the DC values are measured without an input signal.

I hope this will help.

Answer 4

First you need to flip the collector and emitter on the bottom transistor for the circuit to work, but often times you will get this error if there is some very high frequency oscillations in the circuit. The simulator will try to reduce the step size further and further to solve for this, but gives up at a certain point if the time step is too small. This can usually be solved by adding some capacitance to your circuit.

Failing that, a trick that might work (in LTSpice anyway) is to add the directive below. This adds the specified amount of capacitance to every node in your circuit (10pF) in this case.

.options cshunt 10p