IGBT simulation not producing the same waveform, even though the exact same circuit works in LTSpice

So, I am using a 3rd party IGBT model in a larger circuit. And I wanted to switch to QSpice for the increase in speed and to put in some digital logic using C.
I have run into a seemingly basic issue.
I reproduced the exact same test circuit, on LTSpice and QSpice.
I followed the directions to import a subckt file ( copied the text, pasted in the Qspice editor, and selected include entire file ).

The voltage at the collector node of the IGBT, is expected to go from the high rail voltage to the almost 0 (whatever drop the IGBT would have across it).
While the waveform in LTSpice is like that, the waveform in QSpice, goes from the high rail to around 7V.
I don’t know why this issue is happening, but could someone please help me out?
Since it is the same circuit, I had hoped the waveform would also match.

For comparison, first thing you can do is in Qspice : View > Netlist, save into a .cir file
Use LTspice to open this .cir, Run simulation and in waveform viewer compare this voltage node reading.

Hello, thank you for your response.

I tried that out. Got the netlist from qspice, saved it as a .cir. Opened that in LTSpice and plotted the voltage of the same node.

The voltage of that same node is still different in LTspice and qspice. :frowning:

In this case, you can try two more options to see if it can affect simulation results in Qspice

  1. Goto “Preferences”, disable Fast (less accurate) Math
  2. Set maximum time step, for example, “.options MAXSTEP=1e-5”

If nothing change your output waveform, you may want to send this Qspice circuit to Mike through email and explain this situation for him to review.

I tried that out.
Still isn’t working. I’ll email this to Mike.
Thanks for your help. I learnt a new way to debug that I hadn’t thought of :slight_smile:

1 Like

The problem was the way the model was authored. Below is a schematic of the basic internals of the model. Notice that M2 is basically an error. Its substrate should be tied high and it is not. Instead the model shut off the substrate current my setting its emission coefficient to 1,000,000; probably since many SPICE programs can’t handle a zero substrate current. QSPICE does in the interest of support WBG devices which don’t necessary have a substrate or body diode.

Anyway, if you do an update, QSPICE now supports that method of turning off the substrate current and the model should run as intended.