PCB trace width for SMD Fullbridge.

[CM800]

Hello folks,

Im working on a full bridge Motor controller PCB, the problem is the max current going through the traces is 20A. We don't want the board being hidiously expensive however.



Here is the board so far. The problem is the traces i think may be too small for 20A.

The fets i am using only will dissapate 0.5W while on. and since there are only 2 on at any one time (diagonal to eachother) there shouldn't be tooo much heat problems relevent to the fets.

Does anyone have any good tips for high current pcb design? I haven't been doing this for that long.

The actual use of this board is for industrial automation.

Thanks,
Thomas

[Spikee]

via stitching everywhere will increase the overall surface area and lower the resistance thus allowing more current to flow and lower the self heating effect.
 Remove the soldermask of the big fat traces and put solder on it.
 also put the fat trace on the bottom and connect the two with via stitching.
 20 amps is not that hard to do

[max_torque]

20A, with a good heat dissipation (ie, a relatively cool environment) doesn't require tracks that are too big.  Plenty of tricks, like building up traces with sodler, or soldering on extra copper (either laser cut from thin sheet, or i've seen copper "braid"  (like solder wick) used as well.

You can take a stab at the electrical resistance of your trace (plenty of online calculators) and estimate the heat flux.  The important part is to keep the trace cool.  I've done over 400Arms on a pcb trace before (ok, with a back cooled IMS pcb ;-)

Also important will be a low parastic inductance of the parts of the bridge that see high di/dt, to limit voltage spikes and the necessity for active snubbing or slow gate switching etc.  Minimise the distance between the high and low FETS, which also helps limit trace resistance and power loss/upheat etc

As mentioned, using via stitching and multiple layers of copper can help, but for only 20A i don't think you'll have too much of a problem.  It isn't that much more expensive to double the copper thickness on your pcb if you get into trouble with your design either...........

[Alex Eisenhut]

Here's a 120 amp speed controller for a RC car

http://www.soulrc.com/media/catalog/product/cache/2/image/9df78eab33525d08d6e5fb8d27136e95/1/7/1780792_285001618323742_241161390_n.jpg

Granted, they run for 10 minutes and get pretty hot. 20 amps is not a big deal on a bigger board.

You can always download this to give you some numbers

http://www.saturnpcb.com/pcb_toolkit.htm

[poorchava]

You can try to get quotes for 2oz copper.  It shouldn't add too much cost,  but will roughly halve resistive losses in the traces.

[relu]

I think that  the current trace width should sustain without problem 20A, even for 35um copper.
The problem that you have there is the heating of the MOS's. (Those are TO252?)
1/2W doesn't seem that high, but when you don't have any cooling, it might get hot (Ambient + 30C). I would place some thermal vias on the bottom of each mos, and for more ruggedness also route the same signals on the bottom.

cheers!

[CM800]

Thanks for all your replies, im working on the board now and implimenting your suggestions!
I shall post an update when it is done