Mosfet not working propertly

QSPICE
1

Hi,

Could you advise me on what’s wrong with the circuit? The simulation ran, but the MOSFET is not working as it is supposed to.
C3M0032120K_Mosfet_test.qsch (4.8 KB)

C3M0032120K.txt (7.2 KB)

2

The essential problem is that you have mixed up the pin order.

For the .subckt symbol, the symbol pin and the .subckt pin are matched based on their “order” and not their name. Currently, your pin “g” in the symbol actually matches pin “d” in the .subckt, pin “s2” matches to pin “s1” etc., based on their order.

image
image991×474 61.4 KB

In symbol viewer, right click on pin, and you can change PinOrder

image
image553×535 15.8 KB

Finally, be aware that you have to provide a “temperature” (voltage) to either the Tc or Tj pin for this Wolfspeed spice model. They expect you to define the case or junction temperature of this device.

3

If my explanation is still confusing, simply download these files to use.

Wolfspeed NMOS TO-247-4L.qsym (1.5 KB)
Parent.C3M0032120K.qsch (5.8 KB)
C3M0032120K.txt (7.2 KB)

1 Like
4

Thanks for your help. I love qspice.

5

I tried to move forward with the schematic, but it stopped working with a simple half-bridge configuration. The same circuit works well in LTspice but not in Qspice. Could you advise me again on what the problem is?

C3M0032120K.txt (7.2 KB)
DCDC-C3M0032120K.qsch (9.9 KB)

6

Qspice seems not handle this device very well. My personal feeling is that, if a device model built from functions/equations instead of devices, it is quite easy run into timestep too small in Qspice, but not in LTspice.

I changed your circuit to a half bridge configuration, the items that may help include

  1. disable fastmath and to use QSPICE80.exe (.option fastmath=0)
  2. short S1 and S2 of upper FET (0V V1 in this example). I don’t like that, but this seems a way to run in Qspice. If you remove that short, you will see this simulation fail with timestep too small.

DCDC-C3M0032120K-KSK-5.qsch (12.0 KB)

image
image1450×548 60.7 KB

7

Thanks for your support. Indeed, I simulated with the same configuration in LTspice. The Qspice is 10 times slower than LTspice.

Qspice

image

LTspice

image

We made a simple circuit and verified it with actual measurements. LTspice is very close to measurements.

8

To run the exact schematic in 5th post, it seems adding this option can work
Mosfet not working propertly - QSPICE - Qorvo Tech Forum

.option fastmath=0 itl4=100

  • disable fastmath to use QSPICE80.exe
  • increase Transient analysis iteration limit (ITL4) from 10 to 100

But yes, it seems Qspice handle this type of simulation not as fast as LTspice.

By the way, where you generate the difference result between Qspice and LTspice?

9

Each transistor has its own individual chip temperature.
DCDC-C3M0032120K-KSK-AB.qsch (11.4 KB)