SiC models
Banner2

Using Silicon Carbide semiconductor models in 5Spice

At this time, Spice does not have a built-in model for the new SiC MOSFET devices.

Device manufacturers are using Spice’s user defined math equations with (1) custom math functions and/or (2) the DDT function (both part of PSpice syntax) to describe their behavior. 5Spice has been extended to handle (1) and (2) with v2.60 .

> Revised for 5Spice 2.61 <

Using the math functions allows us to get models now, but they are not as forgiving in simulation as a model based on circuit components. They don’t “talk back” to Spice the way its built-in components do. And they simulate slower. They work in operating point, DC or Transient simulation but may not work correctly in AC analysis.

There are no MOSFET semiconductors in these subcircuit models!

October 2016. Things will probably change quickly with SiC models, let us know if these guidelines need updating.

General Guidelines

  • Ignore the guidelines provided for other Spice programs.
     
  • SiC is for power, Spice defaults to IC levels of current and voltage. Run the 5Spice Wizard to reset Spice to your design’s voltage and current.
     
  • DC Bias, Transient at Time=0: if you try to run the device outside its normal limits, such as in breakdown, you may need to select the “operating point” convergence option to get things working. There is no real penalty for doing so, simulation runs a bit slower.
     
  • Transient analysis: Select the “try harder” convergence option. Once you get your circuit working smoothly, you can try turning it off to get a more accurate simulation.
     
  • MOSFET and Diode model selection lists: you will get a warning “5Spice can’t determine the device type of this subcircuit”. Look at the model listing to see if the device type is correct as identified in a comment or by the names of the .subckt terminals. Otherwise it could be something completely different.

Users of other Spice programs:

  • See your program’s instructions for setting ABSTOL and VNTOL.
     
  • Operating Point: in traditional Spice, set ITL1=300.
    however many Spice’s, including 5Spice, have more sophisticated DC convergence algorithms these days - your program may recommend not changing this setting.
     
  • Transient analysis: set RELTOL=0.01, ITL4=100


Technical

  • SiC MOSFETs require much larger gate drive voltages than silicon power MOSFETs.


Company specific

Rohm
You may need to set the Transient analysis "max time step" to be 80% or less of the rise time of the gate voltage. This is to avoid a "time step too small" error.

For MOSFETs, use the power MOSFET symbol in the schematic.

The SiC MOSFET models simulate very slowly.

ST
You may need to set the Transient analysis "max time step" to be 80% or less of the rise time of the gate voltage. This is to avoid a "time step too small" error.

MOSFET subcircuits

name ends in “_V2” have 3 terminals
  Use the power MOSFET symbol in the schematic.

name ends in “_V3” have 5 terminals.
  Use the new NT or PT power MOSFET symbol in the schematic.
  Two terminals are for thermal modeling. Connect a voltage source to the “Tcase” terminal,
  probably 25V represents 25 degrees C.

SCT20N120_V2, SCT20N120_V3  modifications
This subcircuit appears to have a missing connection between drain nodes d1k and dd (connection is present in SCT30N120_V2). This produces huge negative drain voltages or simulation failure. The modification here is our guess at what would be correct, based on the SCT30N120_V2 which is similar but also has significant differences. Use at your own risk.

See “Editing a Model File” below before you start.

    1) find line starting with VLd near the beginning
    2) insert this line following it:    R_kludge d1k dd 1E-03
    Model now works some of the time but fails for other orders of parts in the node list.

    Model uses two Tables that produce node voltages in the pico-volt range,
       a no-no in Spice for a circuit with 1000 volts. Rescale table values to fix this
    3) line starting with G_miller:    delete    “*1E12”
       after G_miller, find line   Ecap alfa 0 TABLE
       delete all the p’s (for pico) from the table entries.
    4) line starting with G_coss:    delete     “*1E12”
       after G_coss, find line   Ecap2 alfa2 0 TABLE
       delete all the p’s (for pico) from the table entries.
    Runs much better. Save file under a new name and enjoy.

SCT30N120_V2, SCT30N120_V3  work in 5Spice

Cree
(note: the Cree C3M series has 3 terminals and is not supported at this time)

Cree C2M SiC MOSFET subcircuits have 5 terminals.
Use the new NT or PT power MOSFET symbol in the schematic. Two terminals are for thermal modeling. Connect a voltage source to the “Tcase” terminal, probably 25V represents 25 degrees C.

Next, the “Die” models have lead inductance of 1 femto(1e-15) Henry which will create poles in your circuit at GHz frequencies. Spice may go very slow to follow them or just go crazy. Use the “Package” version. Graduate to the “Die” version if you are modeling trace inductance or are brave. The ratio of smallest to largest inductance in your circuit should not exceed 1e9 in traditional Spice and 1e13 in 5Spice.

Cree’s SiC subcircuits are a mangling of Spice3 and PSpice syntax, sometimes even in one line. Like mixing English and French. 5Spice rejects a line that mingles the two since it looks like typographical error. You will see an error symbol by the model name in the subcircuit selection list. You need to edit the model file to fix it. not hard.

See “Editing a Model File” below before you start.

1) Lines starting with the letter B
   if you see a double asterisk   ** , replace it with a single   ^

2) In these two lines
  .subckt  cgdmos d2 g
  .subckt gmos d1 g2 s1 Tj Tc

add this to the end:      Params: af=1

3) In .subckt gmos there is a line starting B3.
   In that line there is a parameter named “Adj”
   Place braces {} around the Adj =>  {Adj}

Parameters in lines that start with E or G don’t need braces.

Syntax parents
B lines are Spice3, allowing them to have parameters (enclosed in braces) is Spice3/IsSpice. E,G lines that use the keyword VALUE are PSpice.


Editing a Model File
Use Windows NotePad or WordPad to edit the file. Turn off WordWrap. As a way of working, it's clearest to put an asterisk at the start of the line (makes it a comment line) and then copy that line right below. Modify the copy, then you have the original as reference. SaveAs the file to a modified name. Be careful when you save the file - Windows will append a .TXT extension to the file name unless you select the *.* filter before saving. 5Spice ignores .TXT files in the Library.

Note that Windows hides the .TXT extension by default. Change this in Windows folder settings by unchecking “Hide extensions for known file types” .

IsSpice and PSpice are registered trademarks of their respective owners.

[Home] [Features] [Download] [Register/Buy] [Links/Tutorials] [FAQ] [Contact] [Legal] [Privacy] [White Paper]