There is a thread “PMSM motor Modeling” (PMSM motor modelling) where @bordodynov tells about his LTSpice model collection. I found exactly this model (under “Motors\Ind3phMotor” but for LTSpice), and it is working. I didn’t find any differences that matter for my problem with the “mutual coupling”.
Modification #1 .param Lm=sqrt(Ls*Lr)*k instead of .param Lm=sqrt(Ls*Lr)*k1
Modification #2
B-source does not support current sensing from another B-source in Qspice, i.e., Bm cannot use V=I(Bt).
You need to add a 0V voltage source in series with Bt and sense the current from that voltage source.
However, for some unknown reason, even after making these modifications, Qspice still cannot produce the same results as LTspice. The attached netlist (rename to .cir) runs successfully in LTspice according to the paper, but not in Qspice.
I understand #2, even if it’s not straight forward. But could you pleas explain the the k1 → k thing. I Also have to change the “.param k1=0.97” statement to “.param k=0.97” i guess but why does “k1” is a problem? And if it is, why is “k0” fine?
I tried both modifications and it is running know.
But the result is not like expected (=not matching the results of the ltspice version).
If you or anyone else gets a clue for this, please let me know.
Oh, sorry, I just look into the paper which called to use k, but you changed that to k1.
It seems K is a reserve word in Qspice and give 1.38e-23. I reset .param Lm=sqrt(Ls*Lr)*k1 and Qspice is returning error for using this mutual coupling
Thanks again,
I found one more mistake in my model. The formula in Bx is missing some brackets (it’s “(I(Lb)-I(Lc))” instead of “I(Lb)-I(Lc)”). But it’s still not working fine.
Actually it’s running without error sometimes.
If I’m fresh starting qspice and loading and running my test-model, it returns the error with the mutual coupling. If I’m saving the file (without changing anything relevant) and rerunning it, there is no error anymore and it’s running, but still with another result than in the ltspice version. (This behavior is a little tricky. I tested it several times and sometimes I needed several try’s. And the next time it worked immediately.)
I’ll try to contact Mr. @Engelhardt. There could be some more mistake within my model, but unfortunately there seems to be a problem in qspice as well.
Run it multiple times in Qspice and you will eventually get an error. (Just keep pressing Run after simulation finished). This is what @Thorsten experienced and reported to Mike.
I noticed a strange thing. Sometimes it says: inductive communication is not possible, but if you change the extension in the file to txt and then change the extension back, it counts normally. IndMot3ph3_AB.txt (7.1 KB)
I believe I found the last mistake in my model. I flipped the direction of Lx and Ly. In my opinion this doesn’t match the paper but anywhere: Now (if it’s running*) the results are like the results in LTspice and your QSpice versions with subcircuits.
There are still may simulations ending with an errors, but I’m sure Mr. @Engelhardt finds a way to fix this. I also found the direction dot of the inductors to small and in some orientations it is overlaying the symbol. Maybe this will also be reviewed.
