Announcements

The EV market is bigger and better than ever. Join the EV Webinar to find out how you could best utiilize MOSFET for EVs.

Tip / Sign in to post questions, reply, level up, and achieve exciting badges. Know more

MOSFET (Si/SiC) Forum Discussions

Yilia
Level 1
Level 1
First like given First reply posted First question asked

I downloaded Models of MOSFET CoolSiC 650V from the Infineon official website(https://www.infineon.com/cms/en/product/power/mosfet/silicon-carbide/discretes/imw65r030m1h/?tab=~%2... ), and tried to simulate in Pspice, but an error was reported. The device I am using is IMW65R030M1H_L0. The specific error content is:

--------------- INFO(ORPROBE-3209): Simulation Profile: SCHEMATIC1-TEST ---------------
INFO(ORPROBE-3183): Simulation running...
** Profile: "SCHEMATIC1-TEST" [ C:\Users\Beyond_ice\Desktop\Capture_Simulate\PMGD\pmgd-pspicefiles\schematic1\test.sim ]
Reading and checking circuit
Making index file for library C:\Cadence\Cadence\Cadence_SPB_17.4-2019\tools\Other_Lib\LIB\Simulation_model_silicon_carbide_MOSFET_Gen1_650V_SPICE-update.lib
Please be patient. This may take several minutes...
ERROR(ORPSIM-16387): Missing value
ERROR(ORPSIM-16387): Missing value
ERROR(ORPSIM-16387): Missing value
ERROR(ORPSIM-16387): Missing value
ERROR(ORPSIM-16387): Missing value
ERROR(ORPSIM-16387): Missing value
ERROR(ORPSIM-15113): Model Ld used by X_U8.Ld is undefined
ERROR(ORPSIM-15113): Model Lg used by X_U8.Lg is undefined
ERROR(ORPSIM-15113): Model Ls used by X_U8.Ls is undefined
ERROR(ORPSIM-15113): Model Ld used by X_U9.Ld is undefined
ERROR(ORPSIM-15113): Model Lg used by X_U9.Lg is undefined
ERROR(ORPSIM-15113): Model Ls used by X_U9.Ls is undefined
ERROR(ORPSIM-16015): Unknown parameter.
ERROR(ORPSIM-16015): Unknown parameter.
Circuit has errors ... run aborted
See output file for details
INFO(ORPROBE-3188): Simulation aborted

-------------------------------------------------------------------

I searched for relevant information for a long time but failed to solve it. There was even a post that was very similar to my problem, but I couldn't get a feasible solution(https://community.infineon.com/t5/MOSFET-Si-SiC/Ask-for-the-PSpice-model-of-650V-SiC-Trench-MOSFETs/... ).
I hope to get help from everyone in the community, thank you very much!😊😊😊

0 Likes
1 Solution
Jingwei
Moderator
Moderator
Moderator
First question asked 100 replies posted 10 likes received

Hi,

try to do this: Copy the following code and paste to the model.lib file. Then create a new model, this model should work.

.SUBCKT IMW65R030M1H_L0 drain gate source
.PARAM fpar128=1.1448 fpar129=1.0 Rs=7.39E-04 Rg=4.54E-02 fpar127=6.278
Ld drain dd 2.18n
Lg gate g 9.14n
Ls source s 3.33n
X1 dd g s tech_sicmos_L0 PARAMS: Rs={Rs} Rg={Rg} fpar128={fpar128} fpar129={fpar129} fpar127={fpar127}
.ENDS IMW65R030M1H_L0

BR,

Steven

View solution in original post

0 Likes
6 Replies
Jingwei
Moderator
Moderator
Moderator
First question asked 100 replies posted 10 likes received

Hi,

I got the same problem when i was doing simulation in LTspice. I am trying to figure out internally. 

Thanks and BR,

Steven

0 Likes
Yilia
Level 1
Level 1
First like given First reply posted First question asked

Hello,

Thanks for your reply!

Over the course of a day, I've tried a number of things, but none of them solved the problem. I don't have a clue now, maybe because I don't know how to set and use Lg, Ld, and Ls.
I plan to email the official tech support for help, and hope you can help me if you find a way.

Best wishes,

Yilia

0 Likes
Jingwei
Moderator
Moderator
Moderator
First question asked 100 replies posted 10 likes received

Hi Yilia,

this 650 CoolSiC model are tested with Simetrix. Can you try if it works with Simetrix. We are working on optimizing the SPICE models for LTSPICE and PSpice. They will be published once validated. 

BR,

Steven

0 Likes
Yilia
Level 1
Level 1
First like given First reply posted First question asked

Hi,

Since all the work I have done in the early stage is based on Pspice, I am more concerned about when I can get the device model suitable for Pspice.

BR,

Yilia

0 Likes
Jingwei
Moderator
Moderator
Moderator
First question asked 100 replies posted 10 likes received

Hi,

try to do this: Copy the following code and paste to the model.lib file. Then create a new model, this model should work.

.SUBCKT IMW65R030M1H_L0 drain gate source
.PARAM fpar128=1.1448 fpar129=1.0 Rs=7.39E-04 Rg=4.54E-02 fpar127=6.278
Ld drain dd 2.18n
Lg gate g 9.14n
Ls source s 3.33n
X1 dd g s tech_sicmos_L0 PARAMS: Rs={Rs} Rg={Rg} fpar128={fpar128} fpar129={fpar129} fpar127={fpar127}
.ENDS IMW65R030M1H_L0

BR,

Steven

0 Likes
Jingwei
Moderator
Moderator
Moderator
First question asked 100 replies posted 10 likes received

The logic is change the {Lg} to number.

If you have problem to do this, write me back.

Steven

0 Likes