doAnalyses: TRAN: Timestep too small; initial timepoint: trouble with node "probe_int_probe_int_net-_u1-_on/off__xu1_5_xu1_5" run simulation(s) aborted

Schematic Simulation (Ngspice)
1

image
image1471×522 6.61 KB

I want to sim this ckt but having error “Timestep too small”

2

https://forum.kicad.info/search?context=topic&context_id=60685&q=Timestep%20too%20small&skip_context=true

3

For switched power electronics applications, I usually have to adjust some of the simulations options:

.options method=gear chgtol=1e-11 abstol=1u reltol=0.01 rshunt=1G rseries=0.05 cshunt=1p trtol=1

It’s helpful to look them up in the ngspice manual so you have an idea what you are changing there. Also consider to add a load to the output.

4

Have you carefully inspected your circuit? I’m not sure it should work, regardless of the simulation system. (Check the power symbols, and the on/off and probably everything else including diode models)

5

EDIT: removed, I apologize

6

I think this IC can be setup as an inverting regulator.

1 Like
7

@lucas, you are right, TI datasheet Fig. 8.4.

9

So, I got curious and set up this circuit. I am able do simulate the circuit with kicad/ngspice. The simulation is kind of slow and I cannot verify it behaves correctly. I had to change something inside of TI’s model file though. I replaced all "GND"s with “trickGND”. Otherwise it seems like the IC doesn’t control the output voltage. @holger Is it possible that the GNDs inside the model could be conflated with the circuit GND during simulation? Attached you’ll find my project.

LM2596.zip (13.6 KB)

10

GND is a global node in ngspice and will be replaced by 0 everywhere, except for: add set no_auto_gnd to .spiceinit.

1 Like