EAB450M12XM3 model for Pspice

juzzw123

May I ask where can I get the pspice simulation model for EAB450M12XM3 half bridge power module?

There is a one in all-spice-model package but I cannot run it successfully in Pspice.

Many thanks

Forum_Moderator

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

Bdeboi

EAB450M12XM3.zip

Hi juzzw,

The Pspice compatible models can be found in the 'Pspice' folder from the models download on our website. The all-in-one model is specific to LTspice.

I've attached the EAB450M12XM3 Pspice-compatible netlist here. Please let me know if you have any issues.

Thanks,

Brian

juzzw123

May I ask how can I transfer this cir document to olb & lib correctly?

I tried a way to do the transfer but I still cannot run the model in Pspice.

Bdeboi

CAB650M17HM3_Model.zip

WS_Pspice_ImportGuide.pdf

Hi juzzw,

Here are some brief instructions I've put together for a CAB650M17HM3 model in the past. I've also included a CAB650M17HM3 PSpice model -- you may be able to import that and change the properties to work with the EAB450M12XM3 model.

Thanks,

Brian

juzzw123

Unfortunately, with this approach, I am still not able to run the model.

Could you please help check if there is anything wrong?

juzzw123

Is it possible that we can talk via teams? This is my teams phone number

Bdeboi

Hi juzzw,

Let me spend some time investigating this issue tomorrow and ensure that the model can be imported. I'm mostly curious about the ".ic V 0" line in your error window. Was that line modified from the original model file?

Also, I've just noticed that you are grounding the Tj pins on the model block. Can you try removing that ground connection and trying again? If Pspice doesn't let you float the Tj nodes, try adding resistor between the nodes and ground.

Thanks,

Brian

Bdeboi

Here is what my DPT circuit in Pspice looks like.

juzzw123

Thanks for your support. Now I can run the model in Pspice.

I would like to ask how accurate it is for me to do short circuit simulation or active short circuit simulation with EAB450M12XM3 model?

juzzw123

I run the double pulse simulation for both high side & low side switch with same gate drive configuration.

However the turn-on/off speed of low side is obviously lower than high side switch. Technically with the same gate drive configuration, turn-on/off speed of high side & low side switch should be almost the same.

With Vgson = 15V & totally the same gate drive settings, high side I_gate peak = 2.3A while low side I_gate peak = 1.8A.

May I ask if you know the reason?

Bdeboi

Hi juzzw,

Yes, this is expected behavior due to some additional parasitic inductance on the high-side switch for this particular module. Hope this helps.

If you look at the netlist, you can see the difference between the high side (XQ1) and the low side (XQ2) here:

XQ1 Vd GHI Vp1 TjQ1 IQ1 Mosfet
LcsiQ1 Vp2 Vp1 300.00p
Rcsihs Vp1 Vp 50u
Rcsihp Vp2 Vp 100
XQ2 Vp GLI Vs TjQ2 IQ2 Mosfet

juzzw123

Does it mean high side & low side gate driver configuration (Rgson/Rgsoff or Vgson/Vgsoff) should be different in a real inverter application if this EAB450M12XM3 is used for fastest turn-on/off speed?

If no, then the switching speed is limited by high side however the power loss for low side is not optimal.

Bdeboi

It would be possible to use different Rg's on high side and low side if you are interested in fully optimizing your system. We would also recommend that you validate any conclusions you draw from simulation in hardware by either testing your system or using one of our evaluation kits.

BlakeNelson

Hi juzzw,

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.

Blake