CREE SiC MOSFET C2M0025120D and C3M0350120J

[rintronic]

Gentlemen,

For a simulation at the USB University, we need to use the CREE SiC MOSFET C2M0025120D and C3M0350120J parts, but their Spice models are not compatible with Proteus Spice3F5.

Does anybody know how to convert them in order to be able to use them with VSM simulation and graph analysis?

We have changed the IF with Steps functions, as was recommended for other parts, but keep getting errors with the derivative "ddt..."

I have attached the original Spice models.

Thanks.

Roberto Iglesias

[Ettore]

Unfortunately, ddt is unique function of LTSpice and Cadence PSPICE only and cannot be translated directly and easily in SPICE3.

Anyway, and provided you have translated correctly the IF statements, replaced all .param variables occurrence with their corresponding numerical values, what's following is an attempt - which requires to be tested, though - of ddt function implementation in SPICE3.

Attached you find a schematic solution and the correspondent SPICE deck form. You can call it as an external sub-circuit block, for example XEDDT g1 d3 ddtout DDT or include the 5 lines from C1 to R1 in the sub-circuit that makes use of ddt.

Code: Select all

*   SPICE3 deck form of a DDT implementation
*           INA  INB  DDTOUT
.subckt DDT 1006 1007 1004
* 
C1 1001  1000 1
E1 1004  0    0    1002 1.0
E2 1002  0    0    1000 1.0E6
E3 1001  0    1006 1007 1.0
R1 1002  1000 1
*
.ends DDT

[rintronic]

Hi Ettore,

Thanks as always for your fast reply, we will test this solution as soon as possible and let you know the results.

Regards,

Roberto Iglesias.

[rintronic]

Hi Ettore,

No luck with the simulation in Proteus of the Cree devices.
We have tried everything you recommended and keep getting errors.

I would like to ask you if you please can take a look at the original Spice models of those devices and see if you could translate them for us, in order to be able to use them in the Proteus simulation at the university.

Those guys at the labs made the models work with Mindi of Microchip, according to them is very similar to LTSpice, but we need it working in Proteus.

Thanks in advance for your help.

Roberto Iglesias

[rintronic]

Hi Ettore,

When possible, can you please take a look at those two models from CREE to see if we can have them working on Proteus?

Thanks.

Regards.

Roberto Iglesias.

[Ettore]

No one is here to do the work for you!
What I can do is correcting your model by suggesting further actions to make it (hopefully) working.
If you're unable to translate the model or isn't possible to translate it (may happen) then use a compatible simulator for that particular simulation.

So, in short, post here the model with the modifications you've made so far, the schematic part you created in Proteus and the test circuit the part should work with.

[rintronic]

Hi Ettore,

I have attached the schematic and model used by the student.

Thanks.

Regards.

[rintronic]

Hi Ettore,

Forgot to add the files for the C3M0350120J.

Thanks.

Regards.

[Ettore]

It looks like the last files are exactly the same original unmodified models you have uploaded in the first post.
In order I may try to help you need to carefully make yourself the following changes:

1) The model includes the thermal RC model with two additional pins Tj and Tc (junction and case temperatures).
This means that your part must have 5 pins if you want that model section working properly.

2) Translate all IF blocks using U function as you did for AD8232.

3) Replace all (.param) variables occurrence with the correspondent numerical values as you find it through the model lines. For example: .param p3 = 13, search for p3 and replace all p3 with 13. Also, .param variables in the form .param p9 = {2*p3*p4} must be replaced with pre-computed values. For example: .param p9 = {2*p3*p4} is p9 = 2*13*0.0257 so replace all p9 occurrence to 0.6682.

4) In the Value expression all occurrence ** must be replaced to ^; for example ((V(Tj))**2) must become ((V(Tj))^2).

I'm sure there will be other changes to do as the above modification may not be suffice to make the model working.
Also it is not guaranteed that both models will converge as SPICE solver is substantially different than Orcad PSPICE!

[rintronic]

Hi Ettore,

I will request from the students the modified models they have and also to correct the details you mentioned.

Thanks.

[rintronic]

Hi Ettore,

We have prepared the projects on Proteus 8.12 SP0 for the two Cree models and modified them according to your suggestions to the best of our knowledge.

When you have time please take a look, there is a PDF file in the folder where the graph is shown represents the results we shall see in proteus, once the models work as expected.

Thanks.

Regards,

Roberto Iglesias

[Ettore]

I have modified the C2M0025120D model in order to get it to converge. It is attached here:

C2M0025120D.zip

(21.89 KiB) Downloaded 286 times

Also, I have modified your related test project to be consistent (reason why you put my DDT schematic model between generator and gate is just obscure to me).

Anyway I'm not entirely sure if such the model works as it should or as when simulated in PSPICE. If not then just use a PSPICE compatible simulator (LTspice for example) to simulate this particular device. The C2M0025120D_m is the final cleaned version (without all that messed commented lines in C2M0025120D_1)

About the C3M0350120J I gave up as I'm not sure it can be translated successfully; if you like you may try to modify it yourself using the C2M0025120D model as a reference; I cannot spend much more time on this.

[rintronic]

Hi Ettore,

Thanks for the model and your time, we tested it and it works for what we need at the laboratory.

Certainly, the industry shall unify the use of Spice, in one compatible version, for the benefit of all users.

We will try to modify the other component and if we succeed we will share the result, for your reference.

Thanks a lot again.

Regards.

Roberto Iglesias

[rintronic]

Hi Ettore,

Our student at the Master Degree is developing the model for the C3M0350120J starting from the C2M0025120D model you created.
So far he has cleared all sintax and convergence errors but now a new error is present before starting the Spice analysis and before going back to correct other details, we would like that you take a look at the model.

The error we are getting is this:

Loaded netlist 'C:\Users\ranita\AppData\Local\Temp\LISA1276.SDF' for design 'C3M0350120J version 2.pdsprj'
[SPICE] d:q1:1: breakdown current increased to 0.0134845 to resolve incompatability
[SPICE] with specified saturation current
[SPICE] r:q1:_g: resistance=0, set to 1000
Internal Exception: access violation in module 'SPICEINP.DLL' [00000647].
Simulation FAILED due to fatal simulator errors.

I have included the files for your reference.

Besides that, our student has asked for permission to include you in a paper (essay) as one of the persons who have helped him, just let me know.

Thanks.

Regards.