Good Day,

I am trying to make double pulse test measurements in LTspice by using the spice model of mosfet and gate driver we are using in our actual design but my setup seems to be not working as nothing is appearing on gate of low side mosfet which is device under test. I have used same components which we have used in our actual desgin and the spice models i am using are from infenion but still its strange that my setup is not working. Can anyone here please advise what could be the problem. below is my LTspice schematic. thanks

 

Please post the .asc file and any custom libraries used (.lib, .sub, etc) so we can run the simulation ourselves.

 

LIN on U2 held at GND potential is likely the cause of your problem.
Posting a picture of your schematic is less than helpful. Zip up your project with all of the symbols and libraries and we will be in a much better position to help you.

 

I need to go to work now but will check back. I run this test in the real world. Want to see how your SPICE models work.

 

I agree with PB. You have Lin on U2 grounded, so M2 won't switch on.
U2 needs a forward-biased diode from Vcc to VB, also M2 switching repeatedly, for the bootstrap to work.
M1 gate and source are effectively shorted together by L5, so M1 can't switch on.

 

U2 needs a forward-biased diode from Vcc to VB, also M2 switching repeatedly, for the bootstrap to work.
M1 gate and source are effectively shorted together by L5, so M1 can't switch on.

There are several different tests that can be run in a Double Pulse tester. The most common one turns the bottom fet on twice and does not turn on the top fet. The top one is used as a Diode not as a fet. Shorting G-S on the top fet is just fine.

As stated before, disabling the gate driver is not fine.

 

Good Day,

I am trying to make double pulse test measurements in LTspice by using the spice model of mosfet and gate driver we are using in our actual design but my setup seems to be not working as nothing is appearing on gate of low side mosfet which is device under test. I have used same components which we have used in our actual desgin and the spice models i am using are from infenion but still its strange that my setup is not working. Can anyone here please advise what could be the problem. below is my LTspice schematic. thanks

View attachment 286012

1.The reason why do not see any gate signal is because voltage supply for high side MOSFET is not connected in your circuit. Either you can connect it to a floating supply or generate a supply through boot strap operation.

2. You have connected load inductor across top mosfet. For double pulse test, you need to switch bottom MOSFET to check the commutation of bottom MOSFET.

 

The Gate Diodes are backwards.
As everyone said, missing diode on U2. It does not matter because in this case the top MOSFET is not being tested. ( note the G-S short )
The main power supply is switched open during the test. It is used to charge Cin and during the test the supply is out of the circuit. The power to test the MOSFETs comes from Cin not the supply.

LIN on U2 held at GND potential is likely the cause of your problem.

 

The Gate Diodes are backwards.
As everyone said, missing diode on U2. It does not matter because in this case the top MOSFET is not being tested. ( note the G-S short )
The main power supply is switched open during the test. It is used to charge Cin and during the test the supply is out of the circuit. The power to test the MOSFETs comes from Cin not the supply.
View attachment 286275

I hope you get a big "Thank You, masked man" for those efforts. Truly above and beyond.

 

The Gate Diodes are backwards.
As everyone said, missing diode on U2. It does not matter because in this case the top MOSFET is not being tested. ( note the G-S short )
The main power supply is switched open during the test. It is used to charge Cin and during the test the supply is out of the circuit. The power to test the MOSFETs comes from Cin not the supply.

View attachment 286275

Thank you for your comment. Yes exactly this was the problem that i have mistakenly connected LIN to ground which was causing the problem and now its resolved. now the other problem i have is I wanted to add to diffrent ground potentials in my LTSpice MODEL. one for power stage and second for control signal coming from function generator and gate driver of MOSFET. I am new user of LTSpice so i dont know how can be this done in LTSpice. Can you pls comment how it could be done here? Thanks

 

1.The reason why do not see any gate signal is because voltage supply for high side MOSFET is not connected in your circuit. Either you can connect it to a floating supply or generate a supply through boot strap operation.

2. You have connected load inductor across top mosfet. For double pulse test, you need to switch bottom MOSFET to check the commutation of bottom MOSFET.

thank you fr your comment. What you mean is that i should connect load inductor between Vsw node and ground potential instead of between high side switch and vsw node? also I wanted to add to diffrent ground potentials in my LTSpice MODEL. one for power stage and second for control signal coming from function generator and gate driver of MOSFET. I am new user of LTSpice so i dont know how can be this done in LTSpice. Can anyone here pls help me. thanks

 

I wanted to add two diffrent ground potentials in my LTSpice MODEL.

Two GND symbols on the schematic would have the same potential (0V, the Spice reference). You can have multiple COM symbols (they look like a V) if you need them.

 

I wanted to add to diffrent ground potentials in my LTSpice MODEL

LTSpice recognises only one 'ground' level and all circuits must be referenced to it for the simulation to work/converge. However, there are some tricks you can play. Here, for example is an isolated secondary circuit. Without R1 the simulation will often fail, but assuming typical voltages of a few volts or tens of volts R1 allows the simulation to carry on without significantly affecting the DC or AC operating points. R1 can be replaced with a suitably sized capacitor for AC circuits or even by a DC voltage (with a large series resistor) to fix a ground potential difference.

 

What you mean is that i should connect load inductor between Vsw node and ground potential instead of between high side switch and vsw node?

There are many different types of test that can be done, but for most the load inductor goes to V+ just like you drew.

I wanted to add to diffrent ground potentials in my LTSpice MODEL. one for power stage and second for control signal coming from function generator and gate driver of MOSFET.

A signal generator for a top side MOSFET can be connected as shown. It does not have to be ground referenced.

To look at a signal, like the G-S voltage where "ground" is not at 0V, put the mouse at Gate, push down on the mouse and to not release the button, then move to Source and release the button. The node name is V(N3,N2) which can be hand typed as V(N3-N2). This will show you the voltage from Gate to Source when they are 100s of volts off of ground.

I like to name the nodes. "Gate_top"

 

This is what I use for a floating ground.