[SOLVED] help with multisim simulation

[andreas157]

help with multisim simulation (sim error)

hi, i'm trying to simulate this pfc rectifier in multisim. simulation won't start because of convergence error. tried convergence assistant but also hints on multisim forums with no result :roll:. Tried virtual transistor and diodes. I tried max timestep 1e-3. Nothing. So i guess i'm doing something wrong :-?

Pulse generator is 40kHz. It's a boost converter attached to a three phase recifier. The topology is fine itself. Runs in simulink (timestep 1e-6) but i need a more accurate spice simulation (power losses, efficiency etc).

i got this:

------ Checking SPICE netlist for Design1 - Κυριακή, 10 Φεβρουαρίου 2013, 2:36:17 μμ ------
======= SPICE Netlist check completed, 0 error(s), 0 warning(s) =======
Error message from simulation: doAnalyses: Timestep too small


schematic is

thanks.

 

[FvM]

You shorted part of the rectifiers by incorrect grounding. If the DC bus is grounded, the star point must be floating (respectively connected to ground with a high ohmic resistor to help simulation convergence).

It's not actually a PFC rectifier by the way, because the input currents of a three phase bridge can't be sinoidal.

 

[andreas157]

well, it is actually a pfc converter, the boost converter is meant to work in dcm so that the inductor currents become spikes with a sinusoidal shape (input voltage reference). Filtered out they become a nice sine with a thd of about 10%

hmm. i removed the rectifier's ground. now simulation reaches 4ns and then stops again.

 

[BradtheRad]

1.

Try installing small 'token' resistors in the same wires with the capacitors.

2.

Try installing a token resistor inline with the pulse generator to your mosfet's gate.

3.

Try running an individual ground to components, rather than joining three ends together and then to a single ground.

4.

I see two places where there is a red dot on a wire close to a node, but not on a node. It looks as though wire ends are overlapped rather than directly joined.

- - - Updated - - -

The power-carrying loops might as well be a short circuit during the negative half of the AC cycle.

I have not been able to create a boost converter powered by AC sinewaves. (Although it is possible with a buck converter.)

 

[FvM]

well, it is actually a pfc converter, the boost converter is meant to work in dcm so that the inductor currents become spikes with a sinusoidal shape (input voltage reference). Filtered out they become a nice sine with a thd of about 10%

Yes, not bad for this simple circuit.

 

[andreas157]

the same topology runs ok in orcad. same values, same simulator options (reltol, max step size), even with an output volage pi controller.
i just wanted to use multisim wich is easier to use and most of all, does not crash unexpectedly. But it is weird that simulation does not start...

 

[FvM]

Different circuit simulators have different weaknesses regarding convergence problems. I'm not presently using Multisim and thus can't help with it's specific issues. There are some general points how to avoid respectively find workarounds for popular convergence problems with semiconductor components. I wonder if you have set realistic rise and fall times for the gate driver, at least none are shown in the schematic.

 

[andreas157]

:-D and it's sooooolved! Thanks for that. Rise/fall time were too low. Just increased them and everything is fine! Thanks again!