SiC MOSFET SPICE model not behaving properly

Question

I have been trying to simulate a fully controlled full bridge using SiC MOSFETs and so far haven't gettng at least expected results. So I tried to check what is happening using a single MOSFET and a simple circuit like this -

However, when I run the simulation, the current through the resistor looks like this -

I need to uderstand what I am doing wrong while simulating this circuit.
1. Does the gate need a resistor in series ?
2. The floating terminals of the MOSFET are Tj and Tc (temperatures) I have assumed that they can be kept floating.

Update-
Zoomed in waveform - Edit -
The MOSFET is rated at 1200V and 90A. The simulation works fine up until Vds as ~55V. Thereafter it breaks down and shows these similar results for any voltage above ~55V

Answer 1

The reason it is not giving the results you're expecting is because of your second assumption.

2. The floating terminals of the MOSFET are Tj and Tc (temperatures) I have assumed that they can be kept floating.

The Cree C2M SiC MOSFET PSPICE MODEL Quick start guide REV 1.8 (which was available when I downloading all of the spice models in one zip-file some time ago) specifies the following

The Junction Temperature terminal (Tj) can either be used to read junction temperature or to fix junction temperature. This terminal can be left floating.

The Case Temperature terminal (Tc) must be connected to either a voltage source or a Heat Sink RC Network. This terminal should not be left floating.

The reason is that the electrical and thermal circuits of the model are connected through the device equations. This is true for most SPICE models of semiconductors.

I connected a dc voltage source to the Tc terminal and managed to successfully simulate your circuit in LTSpice IV.

Note: Due to the discontinuities in the models from Cree/Wolfspeed (and others), it is often necessary to modify the simulation tolerances to get the simulation to converge.