Ground plane for flyback

I am doing my first layout for a flyback converter. This is my first SMPS design.
Usually, I have a ground plane on the bottom side of a 2 layer PCB. I haven't seen ground planes in any SMPS designs.
Does the secondary side need a Ground plane?
Can someone explain why.

Hi hithesh,
You can-should have GND planes in SMPS world too, but its more sensitive as some other designs.
You must see for spliting between "normal current" parts & switcher/diode retourns i.e., than by FB & eventually sensing at the load...
Why did you use GND plane in your other designs pls, the same is a reason for SMPS GND-planes too...
K.

You must see for spliting between "normal current" parts & switcher/diode retourns i.e., than by FB & eventually sensing at the load...

Click to expand...

Can you explain a bit more. Are you talking about the secondary side?
Rectification and DC output - One ground
Feedback- another ground.
Both joined to a single point ground.
Is this what you mean?

Yes, so ca. as you are writing.
You can find good apps by PI, TI & ADI...
K.

Hi,
You can read over the most needed basics for good layouting by H. Ott :
http://www.hottconsultants.com/pdf_files/Keynote.pdf
K.

Hi Karesz,

Thanks for the ott article.
I have attached my schematic. I have done the following things-
(Place the critical components close together)
The RCD snubber circuit across the Mosfet and primary inductor.
The diode and capacitor combo at the secondary side.
I have also tried to keep the return path as short as possible.

The manufacture recommends that the traces going to the source pin be kept separate, to avoid noise going into other components. I followed this.
Wouldn't making a ground plane that includes all pins connected to source pin defeat this purpose?

I am not sure what component the ground plane connects to on the primary and secondary side.

On the secondary side, I added a ground plane that includes the secondary inductor pin and all the ground pins - rectifier, filter and part of the feedback ckt.

The datasheet doesn't mention anything about ground plane. But I have followed other guidelines.

Any comments/advice?

Hi,
You see, GND is an issue from SMPS technique & EMC tests...
So from your decription I can imagine your layout: it can be OK, but its only a imagination_you are sended only the schematic...
Datasheets are usually nothing for layout examples_ some time for highest speed OpAmps, ADC-DACs can be that you can see a sample PCB & Schema_ mostly only some text or simple explanations or demonstrations for proper layout/routing...
If have good eyes for details, you will see all needed from PI`s Appl Notes & evaluation boards: i.e. http://www.powerint.com/sites/default/files/product-docs/an47.pdf
http://www.powerint.com/products/topswitch-family/topswitch-jx
Than a SMPS Transformer vendor: http://www.coilws.com/index.php?main_page=index&cPath=2_15
Another relevance are the isolations/crepance distances over PCB!!
You must be care-depending of your countries lows....
Mostly is i.e. 8mm between primary wires/cooper & all secondary metalls to have; included the optocoupler package!! Here is no place for miniaturizing! :-(
Often are the mains parts coated with iso-lacks /ev. covered with an acryle plate...
K.

Here's the layout image file .

From the app note you linked, I will add ground plane from Anode of diode to all the secondary components that have ground.

In the layout, snubber is D2, RDB, RC, CC, C1, back to transformer.

Connections to the source pin are star grounded.

Secondary side -- D3, C4, back to transformer loop to reduce return path.

In some layouts, even the power connection have a broad thick trace, is that really required.

Tnx for your file!
Sorry, I checked it only in very short time, but I would say; change it pls! ...It will fail all safety checks & to right!
D4-A&C has not more distances as 1.5-2mm to the rest of electronics/others said: to secondary parts!!!
Its inpossible near between primary & secondary_you should pull a part of your copmonents, beginning with C6/D4/RF5 & U3_all with so 5-6mm "to left"!!

Than is in your circuit missing the "Y2" capacitance...
The thick traces needed in two aspects:
1,
EMC, a smaller inductance has less problems for you,
2,
Current capability_it has often some amperes of peak currents_ or even more!
I think really; you must to first change these part of PCB/routing.
K.

Karesz,

So you are saying reduce the D4, C6 loop. keep the high frequency current trace less than 5mm and distance between components 1.5-2mm?
It seems impossible. I think I have to put components on the other side.

Hallo Hithesh,
I was not clear writing-sorry...
Read pls new my edited text above these one.

I wished to tell:
you MUST have ENOUGH(& not only max. 2mm!) ISOLATION DISTANCES between primary & secondary parts! It was all...
These is the "Alpha & Omega" of (switched) powersupply designs!

All other aspects as ground plane for some places, or spliting the plains will come only after aprovable placement! Your components are direct omn mains potential, some time plugged as neutral-similar is on D4 & hes areal, others is live on the same components, but both are mains potential, & so dangerous, to separate frome the isolated secondayr!
You must have 2.5KV RMS isolation between both circuit parts_1.5-2mm can not "serve" it for you... :-(
If not others, than the reason is for you important: if somebody will dead in combination of your layouts failure = you will go into a prison_garanted,, I think these isnt your goal!
K.

Karesz,

I moved some components to increase the distance between the secondary and high voltage primary parts. Can you please have a look.

Hi,
I have overseen the U3 befor-sorry, these is to move too_to left w. ca. 5mm (w. RF5/CF3!), than U2 can you move to right w. ca 2.54mm.,& take D4 from place to left from T1, rotated 90 degree & between T1/U1!
C6 is to move to below C1(over D4) too...
Maybe you must shift some to left the U1/RIL/RLS1 compelx too.
Goal is:
You must have clean 8mm distance between primary/secondary parts on the PCB surface or between primary & all coppers/pads form the right side of your transformer, included U3 & U2`s pins1&2!
K.

I moved D4-C6 towards primary.
The U3, RF5,CF3 -- should these be towards the primary too?
what about U2?

I think yes, than others can you not have a creepage of 7-8 mm between all primary & secondary parts...
U2: as I wrote above; 2.5-3mm to right or LPF direction.

Okay. I moved U2 more towards secondary side. I also moved U3 towards secondary side.
CF3-RF5 is now closer to primary side.

OK, I think these with primary separation is OK yet, than all secondary lines/coopers as C4/C5 + & - to D3/LPF & Vout connecting make pls with really thicker/wider coopers!
Only a Via for layers changing between C4 & LPF is surly not reliable(even; if hole diameter is i.e. 1mm)_you can have minimum a double via right side of CPF, I would youse a spetial Via for that (I call PwrVia, with i.e. 0.7mm diameter)!!
D3 likes cooper surface by some higher currents (COOLING)/or minimum wider cooper lines on both contacts...
BTW: whats your output power/current pls?
I would change D1/R1 with CPF_& yet same Via problem as above!! Its place is near to the output connection.I would shift the T1 to top & on the ex place of D4 have a Y2 capacitor_I believe taht you must have it_minimum forseeing is needed! If T1 is moved to top, you can slightly move it to right to (towards C4/C5); than you can have D2 between C1 & T1_with TP4 between both Diodes...
Apropo`s Testpoints:
You have a TP1, between CMC1 & D1, but where is hes reference pls!?
Its not referencable to the primary "GND"(called TP3 in your design)_it NEEDS an EXTRA TP for referencing on the other AC points of D1...
If you have higher current in these design_it need a heatshink on U1 too!
To finish: be care pls with positioning of all "Ref-Designators"!! Momentan are their relative RANDOMLY!_ a programmed failure source for miss populating/ testing on wrong point, needed overtime because you have lot of do to find the physically right component to the schema...
K.

Karesz,

I made some changes.
The output power is 29W (22.5V 1.25A output).
From the data sheet of Top246YN, I don't need a heat sink for this output power.

I increased the traces on secondary side to 60mils. The copper thickness is 1oz.
That should be enough to handle 1.25A.
The feedback component traces are 25mils.
Should I increase the primary side trace width?

I added a ground plane on the secondary side. But I did not add the feedback ckt in the ground plane. The rectifying diode noise may enter the feedback circuit.

Also, the design did not have a Y2 cap. Maybe its not required at this power!

Hali,
I think; these can be good work. I would connect the output GND-Plane NUR! at C4 Minus pole to the output GND_for that you must apply (maybe= depending of your CAD, but relative surl ) some "cut outs" on the other GND PINs or Vias (for only on one point contacting)...
About "primary side trace widths": you can have i.e. 1mm traces(or more), but for your 100mA alone isnt needed_I must tell it so: I would use even 2mm lines...
DONT FORGET pls: The Ref point above existing TP1 (the other AC-in on your D1) is missed too!
A question:
Why dont you like pls a Y2 capacitor!?
Best greetings!
K.