LTSpice error: Time step too small

Question

I am trying to simulate the Buck Converter LM22676 from TI for a 5V output. But LTSpice shows an error saying that the time step is too small when I try to run a transient analysis. Can someone please help me understand what I am doing wrong?

Answer 1

If you tried replicating the schematic from the datasheet at page 14, you didn't do a good job: you missed the output feedback network. And you chose a 1k value for the output load, which is questionable for an output that's meant to deliver 3.3 V @ 3 A; I've made it 1 Ω. Not lastly, C1 and C2 are useless without some series resistance between the supply and them.

That said, the model works, though, for some reason, the output doesn't stabilize at 3.3 V. The soft-start is meant to bring up the output after some 500 µs; the duration is right, the value is not. To be sure we're talking about the same thing, this is the model I used. The symbol is auto-generated so you won't have problems replicating my schematic.

Still, I've made the following modifications (seen in the picture, below), though you may get lucky and not need any:

• added Rser=1m to the bootstrap capacitor
• added Rser=50m to the output filter capacitor
• added Rser=10m Cpar=1m to the input voltage source
• added uic to the simulation card since LTspice has trouble finding an operating point; just start from zero and it will be fine.