SPICE simulation failure

[understress]

I have a circuit that I am trying to simulate. The circuit is a model of a transformer I use (see attached design). If I run the simulation labeled 'Transformer' the simulation runs fine. If I try to run the simulation labeled 'Filter', the simulation fails and the error message is: '[SPICE] TRAN: Timestep too small; timestep = 0: cause unrecorded.'

I have tried moving the earth ground from the left side of the V3PHASE source to where it is now. I have also tried having earth connected to V3PHASE and SEC_2_COMMON connected to earth through a 100M resistor, none of this has helped.

Can anyone shed any light on why this is failing? This is a portion of a larger project that I want to be able to simulate so I can move closer to finalizing the design.

Thanks,

Scott

[understress]

Just to keep this updated: I have added 'IC=0' to each of the capacitors (positive side) and the error message is now: '[SPICE] TRAN: Timestamp too small; timestep = 0: trouble with node SEC_2C_+18VAC_SHIFTED.'

Any ideas?

[Ettore]

... If I run the simulation labeled 'Transformer' the simulation runs fine. If I try to run the simulation labeled 'Filter', the simulation fails and the error message is: '[SPICE] TRAN: Timestep too small; timestep = 0: cause unrecorded.'

It happens as you have configured two different settings for SPICE parameters. The right one (i.e. for simulation labeled 'Transformer') is 'Setting for Better Convergence' which is well suited for High power and/or switching circuits. The 'Setting for Better Accuracy' is too tight for such the circuits; it is better suited for oscillators or when you need to reduce the noise floor in Furier analysis but nothing to do with your circuit. I would then re-load the 'Setting for Better Convergence' for all the simulation graphics and the Animation mode as well.

Additionally, if I were you I would reconsider the value of the coupling coefficient. The value k=0.999 is quasi-perfect coupling coefficient and it's pretty unrealistic for real world transformers with relatively high inductance windings and in particular for such a multi-windings transformers. The coupling coefficient k in real transformers - where the leakage (Ls) is much less than the mutual inductance (Lm) - is approximately : k = 1-Ls/(2Lm). Your transformer would have then Ls=0 which is hard to believe. For middle or middle/high power low frequency multi-windings transformer a more realistic value might range from 0.95 to 0.97.

[understress]

Ettore,

Thanks for that. I did not realize you could have different SPICE settings for each graph. I thought SPICE settings were global to a design. Now I know they are not.

Regarding the coupling value, yes I realize that value was not realistic, it was just a starting point. My transformer is a huge giant beast weighing ~250 kilos (~300kVA @ 10% duty). In the simulations I'm doing, output voltage levels aren't as critical as the phasing is.

Thanks again for the help, I'll keep plugging away.

Scott