Pspice EAB450M12XM3 model temperature dependency

juzzw123

Hi,

The question I have is I cannot see the temperature dependency of this model. The switching speed doesn't change according to different temperature setting in the schematic.

I would like to do switching simulation at several static temperatures so I do the connection w/ the model in Pspice as what is shown in the picture below. 175V DC voltage source means both the highside & lowside junction temperature are 175C constant. If I want chip Tj to be 25C then I will change voltage source to 25V.

Could you please help check if the way of defining the chip temperature is correct?

Could you please help confirm if the temperature dependent characteristic of chip is modeled?

Many thanks for your support.

Forum_Moderator

Thank you for your post, it has been approved and we will respond as soon as possible.

Bdeboi

Hi Juzzw,

Your method of adjusting the temperature should work. However, I am surprised that this works in Pspice -- usually you have to add a small series resistor to prevent a definition error. See my simulation below, I've added 1 uΩ resistors between my voltage source (V5) and the TjQ1/TjQ2 pins. Did you edit the model file to remove the .ic statements? If so I recommend adding them back and using the method below instead.

I have performed a parametric sweep of voltage source V5 and confirmed that the model is showing temperature-dependent behavior. The top plot is the temperature of the Tj pins, and the bottom plot are the Vds/Ids waveforms.

If you want to do a parametric sweep of the temperature (like I showed in the beginning of my post), go to 'edit simulation profile', then under 'Analysis', check 'Parametric Sweep' and define the sweep variable as a voltage source. Here I am sweeping voltage source 'V5' from 25C:175C in 25C increments. This should make it easier to observe the temperature dependency.

Let me also elaborate some on how the temperature of the model works. In typical operation, TjQ1/TjQ2 are left floating, as they are usually used as measurement ports. See the below circuit.

Under this condition, the model will initialize its temperature to the global TEMP/TNOM parameter defined in the simulator. Under 'edit simulation profile', go to 'Options', and you can change 'TNOM' to a different temperature:

I've rerun the simulation with TNOM set to 175C, and with the Tj ports floating. The results are shown below. You can see how the junction temperature now starts at 175C.

Hope this is helpful for you.

Thanks,

Brian

TBhatia

Hi, I hope that this answered your question. I will close this discussion for now but if you have a follow up question, please "Start a New Discussion" and we would be glad to support you further.