Help with LTSPICE Simulation please :)

Thread Starter

selvac19

Joined Dec 23, 2017
26
Hello community!

I am trying to run a simulation but I have been having trouble with the components and their respective outputs. The purpose of the simulation is to verify if the gate driver is adequate for the IGBT model I am trying to control.
The IGBT model I am trying to use for simulation is not the actual component that will be purchased for the definite design.

Gate Driver model: UCC5390SC from Texas Instruments.
IGBT model: IXYH82N120C3 from IXYS

Please let me know any question for clarification. THANKS IN ADVANCE TO ALL!
 

Attachments

ericgibbs

Joined Jan 29, 2010
13,277
hi 19,
It always makes it easier to get help, if non standard LTS models are uploaded with the asc file, thanks.
I don't have time to run the files today, but I am sure others will be interested.
E

@Bordodynov
 

Thread Starter

selvac19

Joined Dec 23, 2017
26
hi 19,
It always makes it easier to get help, if non standard LTS models are uploaded with the asc file, thanks.
I don't have time to run the files today, but I am sure others will be interested.
E
I am honestly confused with the files I uploaded as I downloaded them from the manufacturers website but I see they are not in mod file extension and such. What should I do?
 

eetech00

Joined Jun 8, 2013
2,498
Hello community!

I am trying to run a simulation but I have been having trouble with the components and their respective outputs. The purpose of the simulation is to verify if the gate driver is adequate for the IGBT model I am trying to control.
The IGBT model I am trying to use for simulation is not the actual component that will be purchased for the definite design.

Gate Driver model: UCC5390SC from Texas Instruments.
IGBT model: IXYH82N120C3 from IXYS

Please let me know any question for clarification. THANKS IN ADVANCE TO ALL!
Hi

Try the attached files
I modified the UCC5390 model file so it will work with LTspice.
Also...Use the attached symbol file.

eT
 

Attachments

Thread Starter

selvac19

Joined Dec 23, 2017
26
Hi

Try the attached files
I modified the UCC5390 model file so it will work with LTspice.
Also...Use the attached symbol file.

eT
I highly appreciate your help with this. I have been stuck working on this for months as I was unable to find the proper driver for this IGBT, and now running the actual simulation.
What was the issue with components in simulation?
What was missing so I understand why know it is working as it should :)

Thanks a lot, indeed.
 

eetech00

Joined Jun 8, 2013
2,498
I highly appreciate your help with this. I have been stuck working on this for months as I was unable to find the proper driver for this IGBT, and now running the actual simulation.
What was the issue with components in simulation?
What was missing so I understand why know it is working as it should :)

Thanks a lot, indeed.
Hi

1. While LTspice is compatible with pspice code, There are some device statements that cause issues with LTspice.
I've learned over time to recognize which statements need to be reformatted. I identified those and fixed them.
2. VCC1 sets the expected logic voltage levels at the IN+/IN- pins. VCC1 was set to 5v but the pulse generator was set to 3.3 volts.
The outputs remained off since the input voltage level never reached a high enough voltage level to turn the outputs on.
I set them both to 3.3v.
3. I believe this circuit was derived from design example 11.2.1 on the TI datasheet. The pulse generator wasn't set to 10Khz. I set it to 10Khz.
4. I noticed there were negative going spikes on the trailing edges of the IGBT output pulses. I reset the gate resistors to 10 ohms and that cleared it up. I didn't explore any further why and leave that up to you to research.

BTW- Some spice models will include external device models used to test the circuit.
The UCC5390 model file is such a model and actually includes a IGBT transistor definition in the file. see ".SUBCKT IGBT C G E" line close to the end of the file.

eT
 
Last edited:
Top