Dear members,
I try to make a simulation of PWR050 of TI designs which use the "GA3544-BL ". I know that there is problem in using this transformer and coupling factor. I don't know how to solve it. You can see the sch of the circuit that I want to simulate below:
I will attach the simulation too. Any suggestion would be highly appreciated.
Thanks
Farzaneh
Dear Ulrich,
this is the SCH with the last update. Now I have problem with UCC28600.
I could export a DXF file in orcad and then I convert it to pdf. it's a bit messy and I dont know why it doesn't show everything correctly. I sen you a screen shot of it too.
I wish you can find the problem there.
Also, I think there is an error with iniciating in chip. this is the fault that shows me ORCAD
Thanks
Farzaneh
Hello Farzeneh,
Thank you for the schematic screen shot. Yes, the ORCAD pdf is too messy to view easily. Fortunately the screen shot has high resolution and is very clear.
I have made a copy of it and added mark-ups: 
1. The GA3544-BL has a 2.3mH primary inductance and has turns-ratios of 1 : 0.0158 : 0.158 : 0.079. Working backwards and iterating, I find the actual turns can be 38 : 6 : 6 : 3. The winding inductances reflect from the primary value by the turns-ratio squared, so I marked up the reflected inductances as they should be.
2. Remove C20 from across R25. This cap will distort the current sense signal.
3. Change R4 to 620ohms and connected across pins 1-2 of U4 (as indicated).
4. Change diode D6 to MBRS1100T3. 1N1200 is not a suitable part for this application.
In your schematic, the winding L4 has a polarity such that it reflects the primary voltage during the MOSFET on-time. In other words, it is acting as a forward-mode winding, not as a flyback winding. Is that your intention?
Also, M1 is modeled with 2N6762 which is a 500-V rated FET, and it is a very old part. I suggest to find a modern MOSFET with 600-V rating.
But if it is for simulation purposes only, maybe it will work okay.
Unfortunately, I cannot debug the ORCAD error message shown. I don't know anything about ORCAD.
Maybe if you make the changes that I suggest, the system will run properly.
If it is a timing issue, maybe you need to set a shorter minimum time step for the simulation.
Regards,
Ulrich
Hello Farzaneh,
I am sorry that I am unable to get the UCC28600 PSpice model to work.
I received a similar error message as you did concerning some DIGITAL INPUT VOLTLAGE X$X... at 1.2ns.
I don't know what it means and I don't know how to fix it. No one else around here does either, since none of us are PSpice experts.
Aside from that, there were a number of circuit errors in your schematic diagram, including missing the changes that I indicated in my mark-up above.
I made those changes and I also had to remove all of the diode and FET models and replace them with generic models from PSpice.
I had to replace the optocoupler with a generic current-controlled current source.
Here is a zip-file of my circuit for reference: UCC28600_CKT2.zip
Here is an image of it:
My only suggestion at this point is to try using the TINA-TI model instead of the PSpice, to see if that one will work: https://www.ti.com/lit/tsc/slum608
Modify the TINA-TI file to match the circuit image here.
I hope that simulation will work for you.
Regards,
Ulrich
Dear Ulrich,
Happy new year. I wish you have had nice vacations. I tried to simulate the circuit using TINA. There are some errors that I can't solve as I'm not very familiar to TINA. May I ask you to take a look at it?
I don't know how to model the optocoupler. The other thing is the transformer. i'm not sure if I made it correctly. I used the transformer datasheet.
chrome-extension://efaidnbmnnnibpcajpcglclefindmkaj/www.mouser.es/.../ga3544-463400.pdf
I will really appreciate it
Farzaneh
Dear Ulrich,
I don't know how to appreciate all your effort. I could understand everything you've explained for modeling in TINA. There is sth that I couldn't understand. When we take a look at the transformer datasheet we can see that the "converting relation" (I don't remember the exact name in English, so sorry) is inverse. 
I mean what I highlighted in the photo. I wanna know how you model it in TINA.
Thanks a lot
Farzaneh
Hello Farzaneh,
I believe that "converting relation" translates into "polarity". The polarity of the various windings with respect to each other is indicated with polarity marks.
We often call them polarity dots, too.
Using the above diagram, if a positive voltage is applied across the primary winding (Pri) (+ on pin-1 (the dot), - on pin-2), then a positive voltage will appear at the dotted terminals of all other windings with respect to their non-dotted ends. This also works if a negative voltage is applied to the dot... all other windings will have negative voltages at their dots.
Actually, it does not matter which winding is forced (which has the voltage actively applied), the polarity of all other windings follows the polarity markings.
In a flyback transformer, for example, if winding S1 has +Vout at pin-8 during the demagnetization phase of a switching cycle, then pin-2 will have a positive reflected voltage of Nps*Vout with respect to pin-1.
In the TINA model that I sent to you, I did not know how to use a non-linear model so I used the Ideal Transformer model. Also, I do not know how to add more windings to the model, so I just added several Ideal Transformers with their primary windings connected in parallel. Since the Ideal model has infinite primary inductance and zero leakage inductance, I added those parameters as lumped elements. Lm (at 2.3mH) is across the ideal primaries and Llk (at 17.6uH) is in series with one of the primary leads. The specific turns ratio for each secondary winding is entered at N2, where N1 = 1 in all cases.
Even though some of the polarities are not shown as "inverse", you can connect the external circuit to get the same effective inverse polarity.
For example, the VAUX winding (P1) will have pin-3 connected to primary GND, and the AUX diode connected to pin-4.
I did not add winding resistances or capacitances or core loss to avoid making the model too complicated. Some or all of that higher-level detail can be added later after the simulation is running properly for the normal input and output conditions.
Regards,
Ulrich
Hello Farzaneh,
I was able to obtain some help form a colleague more knowledgeable than me and he made some modifications to the system model and certain settings.
Here is a working model, although it is not optimized, it does converge and run: UCC28600_trial_for_Farzaneh.TSC
Here are three Analysis settings that he changed; all others are default:
Here are example screen-captures of his simulation results:
Aside from the Analysis settings, he changed several of the semiconductors and a few component values.
Unfortunately, he deleted the disconnected circuits. I suggest to run this working model and make changes to improve its transient performance first, before adding the other circuits back in.
Regards,
Ulrich
