LT-SPICE blows up when I sim this. Any ideas why?

[ModernRonin]

Someone on Reddit posted a question about a PWM circuit using a 555 timer.

I was getting screwy results (max current 1.4mA) when simming his circuit using the generic nMOSFET, so I replaced it with an IRFP4668. Nice bog-standard mosfet, I thought.

Now the simulation is hanging up and never finishing. It seems like it always goes insane when the transistor switches on for the second time. (First switch-on is fine.)

Here's the LT-SPICE file: http://www.gully.org/~mackys/crazy.asc

Any ideas what's going on here? Am I doing something wrong? Is LTSPICE just screwed up in the head?

[lamja]

Hi.

If you change your L1 from 10 (H) to 10m (mH) it works just fine... Are you sure it should be 10H?

I often get this problem, but changing some value (extreme high or low) usually do the trick.

R6 and C4 looks like they have no purpose.

[Zero999]

This is a classic, I remember doing a simulation of a circuit with a 10F super capacitor and was wondering why it wasn't working, until I realised that Spice is case insensitive and it treated 10F as 10fF which is 10×10^-15F and is probably less than the capacitance between the pads for an 805 SMT resistor.

[jahonen]

General rule is that you never enter a unit in component values in SPICE. That helps to solve most stupid mistakes. Only killer feature are prefixes m and meg, where m = 10^-3 and meg = 10⁶. Or, alternatively use the exponent notation, 10k = 10e3, 1 M = 1e6 etc.

Regards,
Janne

[ModernRonin]

If you change your L1 from 10 (H) to 10m (mH) it works just fine... Are you sure it should be 10H?

I'm sure. It's a 2.5 HP, DC electric motor. 18.5A @ 130V.

R6 and C4 looks like they have no purpose.

You're right, they don't. I was just fooling around there. Taking them out doesn't change the sim blowing up, though.

[ModernRonin]

Thought the 555 might be causing some sim weirdness, so I took it out and put a voltage source configured for PWM in there instead. Still blowing up:

http://www.gully.org/~mackys/crazy2.asc

[jahonen]

Try changing the solver to "Alternate", seems to run much better than the normal solver. (Simulate -> control panel -> SPICE -> Solver = Alternate). MOSFETs seem to be difficult for the simulator sometimes.

Regards,
Janne

[ModernRonin]

Beauty! Thanks a lot!