SpeedFit™ Design Simulator
Simulate and evaluate the performance of SiC-based power circuits and determine the right SiC device in seconds.
Start a SimulationTemperature nodes on the new SiC module LTSpice models
For the new SiC module LTSpice models, is there thermodynamics involved ?
How to you interpret the nodes 'TjxSch' and 'TjxMos' where x={H,L} ?
Are these temperature in deg C ?
Can we get some user-documentation for these models ?
Also, how to get the latest version of the models - specifically the CAS175M12BM3 !
Comments
-
Hello, thank you for your message. A member of our technical team is looking into your questions and we will respond shortly.
-
Hi C1Ron,
Our LTspice models are in development (i.e. subject to change between now and launch) and we are engaged in accepting feedback from customers. For now, we are providing them on a case by case basis, but we will launch our new model library later this year. At that time, we will have documentation and user guidance available for these models. That said, here is the model you requested:
To your more specific questions, the models have electrical dependence on junction temperature (Tj), and their initial temperature is set by "TEMP" (LTspice's default temperature parameter). Like TEMP, all Tj/Tc in the model are in °C. The Tj will also reflect transient changes as there is a cauer network in the model (which is fit to the Zth in the datasheet) for each switch position. TcH and TcL are the case temperature ports to model your external cooling system. If you would prefer a static Tj instead of the closed-loop thermal model, you can set "Thermals=0" in the first spiceline (right click on the model to edit), and the cauer networks will be bypassed. The electrical parameters will still vary based on your definition of TEMP.
Finally, the distinction between TjhSch vs TjHMos is Schottky diode vs MOSFET junction temperature (for high or low side). The Schottky ports are not relevant to modules which are MOSFET only (e.g. CAB450M12XM3), but are necessary for our parts with integrated Schottky diodes (e.g. CAS175M12BM3) since the diodes are different pieces of SiC with different thermal characteristics than the MOSFETs. As a helpful note, the third letter in our part numbers shows B for MOSFET only, or S for integrated Schottky diodes. This raises the question, why leave the ports for models without Schottky diodes?
The benefit is that I can simply change the part number in the model, and change to a different model file in the library. In fact, the file shared above is precisely the same one given here, https://forum.wolfspeed.com/discussion/453/thermal-properties-for-eab450m12xm3#latest, with only the part number of the model changed. If you change the part number yourself, you will get "Unknown subcircuit" errors for models that are not yet in the library (notable modules missing from this version are 1700V devices and Wolfpacks, which will be added prior to it launching the library on our website). Additionally, if you looking to simulate WAS175M12BM3, please use the CAS175M12BM3 model, as it is electrically and thermally equivalent.
I hope that fully addresses your question!
Blake
-
Hi, I hope that this answered your question. I will close this discussion for now but if you have a follow up question, please "Start a New Discussion" and we would be glad to support you further.
