How to Simulate Silicon Carbide Transistors with LTspiceMarch 16, 2020 by Robert Keim
This article reviews the silicon carbide scene and then explains how to get SiC SPICE models and incorporate them into a simulation circuit.
Silicon carbide (SiC) is an increasingly important semiconductor material, and in fact it may eventually displace silicon as the preferred technology for high-power applications. An existing AAC article by Robin Mitchell provides a good overview of SiC, which discusses the material’s history and advantageous characteristics, summarizes its evolving role in the electronics market, and points out challenges to widespread implementation.
If you’d like to see some detailed information on one particular SiC switching device, you can refer to AAC’s article on the C3M0075120K. This N-channel FET is manufactured by Wolfspeed, which is a familiar name in SiC technology and also the supplier of the SPICE models that we’ll be using in this article series.
Driving SiC FETs
One factor that complicates the transition to SiC-based solid-state switching is the drive requirements, which differ from those of silicon MOSFETs or IGBTs. Furthermore, a carefully designed (and somewhat complex) drive circuit is required to ensure that an SiC device lives up to its full potential. Here are a few prominent aspects of SiC gate-drive circuitry:
- Large positive gate-source voltages (around 20 V) are required, and the gate voltage must be pulled below ground when turning off the device. You’re looking at a control voltage that should be able to swing between +20 V and –5 V.
- The gate driver must be able to source a lot of current and sink even more than it sources. This app note from ON Semiconductor recommends “several amps” of source capability and at least 10 A of sink capability.
- The gate driver must also be capable of producing rapid rising and falling transitions.
Don’t let this discourage you, though, because SiC offers major benefits—reduced switching losses, higher-temperature operation, lower on-state resistance, etc.—that are well worth the extra effort in some applications.
The UCC21750 from Texas Instruments is an example of a gate-drive IC that is compatible with SiC MOSFETs. This diagram of a three-phase motor-control application is from the device’s datasheet.
SiC SPICE Models
Circuit simulation is an extremely useful tool for design, analysis, and general electronic edification, and it’s freely available to engineers everywhere. If you’re interested in incorporating the benefits of silicon carbide into your projects but are feeling unsure about the various operational differences and implementation details, simulation might be a good place to start. Simulating some test circuits is also a great way to gain familiarity with SiC devices.
In this article, we’ll be using LTspice to work with SPICE models supplied by Wolfspeed. Wolfspeed offers models for SiC N-channel FETs and SiC Schottky diodes. The models are compatible with PSpice as well.
You can download the files here. (Be advised that you do have to fill in some information, but then you get immediate access.)
You’ll need to copy both the symbol files (these have the .asy extension and are in the “LTspice Symbol” subfolder) and the model files (.lib extension, not in a subfolder) into your LTspice installation.
There are four FET symbols; one is for bare-die devices, and the other three are for packaged devices with different pin counts.
Copy the .asy files into LTspice’s “sym” directory. I created a new folder, such that my .asy files are in “C:\Users\...\Documents\LTspiceXVII\lib\sym\WolfspeedMOSFET”; the separate folder makes the components easy to find when you want to add them into an LTspice schematic:
The .lib files are text files that describe, using the SPICE “language,” the electrical behavior of a particular device. For example:
This is the SPICE “model”: it contains mathematical relationships that approximate the electrical behavior of a component. And actually, the SiC models from Wolfspeed also incorporate temperature information; we’ll explore this feature in a future article.
I copied all of the .lib files into a “Wolfspeed” folder in “\lib\cmp,” like so:
Circuit Simulation with SiC Models
Adding one of the Wolfspeed silicon carbide MOSFETs into an LTspice schematic is a two-step process. First, you add what is essentially just a symbol. Based on the number of pins of the part that you want to simulate, you’ll choose one of the four symbol options mentioned above:
Let’s say I want to test the C2M0025120D. I check the datasheet and see that the part is in a package (i.e., it’s not a bare-die device) and that the package has three pins. Thus, I choose the “nmos_TO247_3L” symbol.
Once the symbol is in the schematic, it serves as sort of a generic carrier for the SPICE model corresponding to the specific device to be simulated. Thus, you need to tell the symbol which part number you want to use by right-clicking on the FET and filling the “Value” field with the name of the part’s library file (without the .lib extension).
If at this point you design a circuit and run a simulation, you will get an “unknown subcircuit” error. To allow LTspice to use the model that is called out in the FET’s “Value” field, you must identify the library file using a .lib command. You can include a full path (in quotation marks), but LTspice will automatically check the “\lib\cmp” directory first, so if your .lib files are in the “\lib\cmp” directory, you can just specify the subfolder and the filename. My .lib command looks like this:
Here’s an example of a circuit that is ready for simulation:
Simulations can be very helpful when you’re trying to incorporate new components into your designs, and this approach is particularly effective when manufacturers supply part-specific SPICE models. We’ll continue working with SiC MOSFET simulation in the next article.