I’m looking at EPC GaN devices and they have both LT and Pspice models available on their website. Which would be recommended to use in Q, LT or P?
cheers
Hello @ChrisHew If you post a link to where you can get those models I will give them a try and report back 
Update: Since you never posted the link I had to go find some EPC spice models myself, not sure if they were the same ones you were looking at but the LTspice models imported and worked just fine.
Here is the link, sorry got tied up with some other things.
thanks.
I’m just wondering if i should be using the LT model over the Pspice models, or maybe it doesn’t matter?
For EPC2304, EPC only provided a sub-circuit model for its Pspice model but with example in LTspice model. I didn’t spend time to study their different, but as LTspice model with example, and its library latest update is 03/07/2024, I just simply take this library for comparison with Qspice.
Just a remind, LTspice library EPCGaNLibrary.lib consists of many EPC GaN subckt model, the most easy way to use it is with .lib directive. Of course, you can also just copy a subckt and use Qspice auto symbol generation. But I just made a generic symbol for the purpose of using it with .lib directive.
In addition, EPCGaNLibrary.lib missing a .ends for EPC2361, LTspice can accept such error but Qspice doesn’t. You have to add .ends at the end of library file for Qspice to accept it.
On the other hand, its LTspice example Example EPC2001.asc has syntax error in V3 and V4, which will not run in LTspice v24. In below example, I modified V3 and V4 pulse description for this example can run in LTspice for comparison.
Here is a generic symbol for ECPGaN (sorry I didn’t draw the body diode as just copy from my other generic NMOS symbol, and I would like its pin direct match default NMOS position, so it is not exactly follow a common MOSFET or GaN with gate closer to source pin), the library with .ends included and renamed into .txt, and an example which equivalent to the example in LTspice (LTspice doesn’t display its Rpar and Rser in default, but LTspice example did have that and I add into Qspice example)
One thing I love to point out is that, LTspice needs ~12s to run this simulation but Qspice only needs 2s, which is why Qspice is superior.
ECPGaN-Generic.qsym (896 Bytes)
EPCGaNLibrary.txt (310.6 KB)
Example EPC2001.qsch (10.2 KB)
1 Like
EPC has updated its EPCGaNLibrary.lib on its website. The LTspice example has been updated as well and can now run on the latest version of LTspice. The library file has also been corrected, with the addition of “.ends” in its last model. This means that the library can now be used in Qspice directly without requiring any syntax corrections.
Therefore, the previous message is outdated, but the concept of using the EPC LTspice library in Qspice remains valid.