Copper pour right under Flyback isolation transformer

Status
Not open for further replies.
C

cupoftea

Advanced Member level 6
Joined
Jun 13, 2021
Messages
3,059
Helped
62
Reputation
124
Reaction score
139
Trophy points
63
Activity points
15,963
Hi,
We have covered totally under the Flyback SMPS transformer with secondary ground copper, and primary DC ground copper.....on layers 2 and 3 repsectively....so it doesnt matter that they overlap each other in the isolation barrier.
We had to do this shielding as there is an earthed enclosure 5mm under the PCB, and we need these copper pours to shield the emissions from the transformer from getting into earth.

But we've been told its not allowed...why?...its internal layer copper.
 

Sort by date Sort by votes
Capacitive coupling from transformer to the earthed heatsink......kind of the radiated emissions from the transformer also propagating to the earthed heatsink.
 

Upvote 0 Downvote
...For a 1.6mm PCB, ayk, the prepreg will be some 0.35mm thickness....thats good for many kV.
Ayk, in air, flashover distance is 160um per kV......so going through pre-preg it will be much more forgiving.

Page 53 of the below IPC-2221A, ayk, the bastion of all things PCB layout, confirms that for internal tracking on PCBs, you can get 301-500V with just 0.25mm on the same internal layer.
As such, if you are on two different internal layers, then the clearance will not need to be high at all....it certainly wont need to be 6mm for pri to sec clearance.
I do believe that IPC-2221A does not specify an "internal layer to different internal layer clearance" for primary to secondary clearance........but it is up to the maker to use due diligence....could you agree?


IPC-2221A PCB standard
https://www-eng.lbl.gov/~shuman/NEXT/CURRENT_DESIGN/TP/MATERIALS/IPC-2221A(L).pdf
--- Updated ---

The following claims 54kV/mm for pre-preg
https://www.isola-group.com/wp-cont...s/185hr-laminate-and-prepreg.pdf?t=1005241780

...As such, i think we will be ok with our 3.5kV regulatory flash test...would you concur?
 
Last edited:

Upvote 0 Downvote
For HV PCB, you'll often design a specific stackup according to isolation requirements rather than using standard stackup.

IPC-2221A states in the first lines of chapter 6.3 that the B1 internal clearance requirements apply for vertical isolation.

I prefer to refer to IEC 61010 for internal PCB clearance, it specifies the isolation requirements more detailed. Other than IPC it's a safety standard with complete test specifications.

Your post mixes breakdown and working voltage specifications which can't be compared. The relevant parameters for insulation design are working voltage and intended isolation type functional, basic or reinforced.
 
Upvote 0 Downvote
Status
Not open for further replies.

Similar threads

Menu
Log in
Register
Cookies are required to use this site. You must accept them to continue using the site. Learn more…