PCB layout recomendations for a fllyback transformer

[MechEng87]

Hello,

I am working on a design for a flyback transformer circuit based of an LT3750 EMS and a Coilcraft DA2034-AL Surface mount flyback transformer.  My current design has the the small LT3750 (MSOP-10) and most of the control componenents ie. resistors and caps on the bottom side of the board and are directly underneath the primary side of the transformer.  Does anyone have any experience with this kind of a setup and will I run in to possible problems with EMF or, the bottom tracks having induced noise from the 100khz to  300khz operation that the LT3750 supposedly operates?  I'm going for a small form factor as possible so that is why I'm mounting the control chip where I did but can obviously move it if it is generally a bad idea to mount stuff on the bottom of transformers like that.  I've got my Schematic and PCB layout pictures attached for reference.  My design is basically straight out of the app notes for the datasheet of the LT3750.

Thanks everyone

[floobydust]

I will give my observations, not that they are right or anything. Taken with a grain of salt.

It is important to have the high current loop done well, as LT mentions.

R12 return to GND terminal should be dedicated, having it's own pour or trace. Right now, R12 currents add noise to C3 and all the right-side GND pour there.
I would move everything up and have a dedicated pour connecting R12 right to the GND terminal and C4, C5, and all other GND pour isolated with a slice. Like a fork or "Y".

Pin 3 CHARGE should be tied to VCC? Usually run that like pin 1, 4 (jut out) instead of directly between pads so the PCB house does not mistake for a copper bridge.

I do not see thermal reliefs on the PCB top (red) but do for the bottom layer. It will be very hard soldering the transformer, caps etc. to get enough heat there.

I suggest a (flyback) HV output capacitor on the board, even a little one. Otherwise it will be a very noisy wire connecting to HV OUT and interfere with other hardware. Where are your output caps and bleeder resistor?

The MOSFET drain connection is med. voltage (<100V) very noisy so I would have no pour under the transformer to the feedback via, just need a thin trace connecting to the transformer. Best to keep the gate trace a bit further away from it (drain) instead of alongside.

The transformer emits electrical noise from it's windings and you have nothing to shield the IC. The underbelly of the transformer can "see" your IC and traces.
Under the transformer I would have a GND pour to shield the E-field from the transformer windings from radiating onto the IC.

I put an LED on something like this so I know it's running and hazardous, for safety.

The 56uF 25V caps are spec'd as polymer types, but you have a boxed footprint. 100uF seemed more popular and LS=2.5-3.5mm check sizing.

I think the IRF540 (100V 28A 7.7m) is oversized and you could save a lot of room there. PHT6NQ10T (100V 3A 90mR) is SOT-223 part LT gives as an example.

[MechEng87]

Thanks a lot for the design considerations, I will make some changes as suggested.

I do have some questions, the GND pour you suggest under the transformer to shield the underside, should that be completely isolated from any other pour? Or should I have it tied to the rest of the GND through a small trace to connect it to GND?  The thermal reliefs I removed from the top pour for current handling considerations but if this is unwise due to manufacturing considerations i will add them back in.  I have gone with a different MOSFET, an ON SEMI FDS5672 which appears to have similar characteristics from the datasheet.  I agree having thought about the design to have a small flyback cap on the output of the transformer, as the main caps are on a separate board with their own bleeder resistors.  I will add a small one to this board and add a second bleeder resistor and some indication that there is an active high voltage circuit working, like a led as suggested.  Having some feedback here really helps.

Thanks!

[MechEng87]

Thanks for all the suggestions,  I updated the PCB and schematic to what i think is an improved design. I also added some high voltage isolation slots between the primary and output of the transformer and between the output cap.

[MechEng87]

Could this be improved by simply widening the board to allow a thicker gnd pour along the  lower section of the board?