Pulsed power

[pulsed_power]

I was wondering if Multisim was suitable for simulating high voltage pulsed power systems. I am still quite new to the software and I have some convergence errors in a set-up I tried to do a transient analysis on.

I have attached a picture of the circuit. The capacitors have an initial voltage of 10kV and are discharged into the inductor once the SCRs (Ignitrons in real life) are triggered by the pulse generators.

I would appreciate any advice.

Thanks!

[Mahmoud_W]

Hi,

I have done high voltage simulations and the results we quite accurate.

Can you please send me your circuit to see why it's not converging.

Hopefully I'll be able to help.

Thanks,

Mahmoud

[_user32]

pulsedpwer,

I observed the convergence issues:

To adjust to make run, I had to adjust a few circuit configurations - please check to see if these adversly impact the design or not:

1. 2 back to back capacitors are never a good idea without a small amount of resistance.   (Note in v12 you can use the advanced Cap or Inductor parts - which are more realistic.)   I added a small 1Ohm resistor on each Cap.

2.  I grounded your Pulse voltage source generator.

I also changed the SPICE engine settings (Simulate -> Interactive Simulation Settings)

1. I adjusted the default Time Step (TMAX) to something on the order of 1E-9 (to account for pulse rise times)

2. Analysis options -> SPICE options (custom settings)

     a. I adjusted RELTOL slightly wider (0.005)

     b. I changed Transient integration method from Trapezoidal to Gear (better for pulsed waveforms)

     c. Changed RSHUNT to a smaller value (in case there were any nodes within the SCRs where charge was accumulating)

Please try out these changes in your own design...    Not sure what nodes are of interest but I setup my circuit with a current probe and voltage to a scope...

Regards,

Pat N

[SiLRing]

Hi pulsedpwer,

If you are new to SPICE simulation you may find a couple of resources helpful to further understand how to deal with convergence in power circuits.

http://zone.ni.com/devzone/cda/tut/p/id/13714#toc3

and

http://zone.ni.com/devzone/cda/tut/p/id/5579#concepts

Could help you to work with your circuits in Multisim.

Regards,

Shauna R

[pulsed_power]

Thank you everyone for spending time and helping me.

The changes _user32 suggested do in fact help the circuit converge.

The references posted were also very helpful.