# LTspice Hung Up For Certain Voltages?

I am running a transient model of a Type-E PFN circuit (probably not an important detail) and my processing time jumps from about 1 minute for one DC source voltage to roughly 475 years for another.

My circuit basically charges up a series of capacitors and switches the voltage into a resistive load at 1us.

Here is the jist of the circuit that I am working with:

When I set the voltage to 100k the model runs with no issue as seen here:

However when I set the charge voltage to 80kV the model hangs up at ~2ps and the processing time drops to something like 1 fs/s wich will never finish.

Does anyone have any idea why the charge voltage would effect the model? It works for 30k, 50k, 100k and scaled values (i.e. 30V, 50V, 100V), but does not work for 70k, 80k, etc.

THANKS!

edit: Here is another view of my circuit (it is too large to show the whole thing):

It consists of 4 stacked versions of the first picture to multiply the voltage. I am relying on the DC operating solution to generate a floating voltage on my capacitors in the PFN (so I can't use uic I think). I found that I cannot use .ic for these voltages because they will all be ground referenced and the model wont work.

• Is V2 directly connected to ground, or floating? If floating, it may help adding Rser (some small value, even 1 would work given your other element values). You could also try to add vt=2.5 vh=-2.5 (a negative hysteresis) to the switches' .model cards. Also, you could just specify Rser for the inductors, to reduce the node count (e.g. {L_coll1_A} Rser={Rind1_A}) and, while you're at it, also add some (not too) large enough Rpar (tens/hundreds kOhms). The caps could also use Rser if the changes are abrupt. Also, avoid .ic for inductors, better use uic in the .tran card. – a concerned citizen Dec 14 '17 at 6:53
• @citizen I tried adding a series resistance to V2, but it hangs up my model in the same manner as mentioned above. Also I rely on a DC operating point solution to charge my capacitors while maintaining source isolation so I don't think I can use the 'uic' modifier (correct me if I'm mistaken here). Thanks for the pointers though! I'm trying to clean up my style, and I really appreciate the tips. – Nick Kallas Dec 14 '17 at 16:02
• If you only add Rser=0 it does nothing. The reason is that, given LTspice's working with matrices, voltage sources that are not directly grounded may have convergence issues. Adding Rser makes LTspice internally convert the voltage source to a current source, which has almost guaranteed convergence. You're right about the uic, I didn't know how you want it. One last tip: for coupling, LTspice considers 1 to be 0.9999... and, rarely, it has been found to create problems, so you could also try to make the coupling 0.9999 or so (which should be fine, even from an ideal's POV). – a concerned citizen Dec 15 '17 at 6:20