1
\$\begingroup\$

This is the first time I've ever designed a power PCB/ a PCB that needed to take a high current, I'm looking to check that I'm doing this right and for any advice on how to improve? details below.

I'm using an arduino to control a 300W film heater in a PID loop kind of thing, and using a MOSFET to switch the high voltage which the arduino can't supply.

Given that it's a 24V supply and the heater is 300W, this trace needs to support 12.5 amps of current. If I have a PCB with 1oz/ft^2 copper thickness, this means a pretty manageable 5mm ish trace width - I narrowed the trace going into the MOSFET terminals because otherwise it wouldn't fit - is this going to be a problem? Image below:

image of current PCB layout

Edit: The MOSFET I'm using is the IRLB8743PbF, and this is the circuit schematic:

circuit schematic

\$\endgroup\$
3
  • \$\begingroup\$ How the arduino ground and supply interact with the 24 volt supply and ground is important detail not shown. Not indicating the MOSFET is also something that makes answering this properly impossible. \$\endgroup\$
    – Andy aka
    Commented Sep 18, 2019 at 10:03
  • \$\begingroup\$ Is there a reason for why everything is placed so far from each other? \$\endgroup\$
    – Harry Svensson
    Commented Sep 18, 2019 at 13:14
  • \$\begingroup\$ @HarrySvensson just figuring things out so havent thought much about positioning yet :) my current version is much more compact \$\endgroup\$
    – Amy Fawcett
    Commented Sep 18, 2019 at 13:38

1 Answer 1

Reset to default
1
\$\begingroup\$

If you can i'd move the input connector to next to the output one, since the input_1 trace can go directly between the two. That'll shorten the trace lengths between the connectors and to and from the MOSFET. I'd also copy the traces to the front and back of the PCB to maximise the copper carrying current and look at necking down the traces a little less (depending on what the board house can manage).

If you're copying the traces to the front and back of the PCB then you don't really have to take any chances with minimising clearance. One final tip for this kind of situation is staggering the drain and source pins so they can be necked down less but this is trade off between between the gain and current loop area by having to stand the MOSFET further away form the PCB to do it.

\$\endgroup\$
9
  • \$\begingroup\$ If i copy the traces to front & back of the PCB, does this reduce the necessary trace width? or is it just to make it more stable? also, if i do this, do I need to add any vias or something? I feel like i've read about this technique on other threads but not understood it. (thanks so much for your help!) \$\endgroup\$
    – Amy Fawcett
    Commented Sep 18, 2019 at 10:36
  • \$\begingroup\$ @AmyFawcett - Your goal should be to get as much copper as possible in the shortest possible distance. The suggested duplicating the traces on both sides of the board is aimed at that goal. As a result consideration to reduce trace width should not be in the discussion. I do not see any need to add stitching vias in this case due to the fact that both your connectors and the MOSFET are already through hole parts. \$\endgroup\$
    – Michael Karas
    Commented Sep 18, 2019 at 11:12
  • \$\begingroup\$ I'd agree with @MichaelKaras in that filled vias are not really needed in this case. If you were switching at high frequency with high dv/dt then it might be time to start discussing what paths current will take but for now you don't need to worry. I'm also presuming you are PWM'ing the MOSFET and heat-sinking it well as a quick inspection of the SOA graph suggests you're going to be operating well beyond the (usually quite pessimistic) DC limit of the device. \$\endgroup\$
    – hooskworks
    Commented Sep 18, 2019 at 11:33
  • \$\begingroup\$ If going two-sided, is it possible to have a "fat" connection to each terminal on alternate sides of the board, and a thin one only on the other side, iyswim. At the moment the neck widths are limited not only by the pin separation but also the other incoming trace. If the traces narrowed to a neck only on one side of the board (a different one for each of the two traces), you would only have to worry about pin-separation. I don't know if this would work in terms of soldering to the through-hole device. Is there enough of an electrical connection on both sides of the board for this to work? \$\endgroup\$
    – Dannie
    Commented Sep 18, 2019 at 11:53
  • \$\begingroup\$ @hooskworks as in, I'm going to need a better mosfet? \$\endgroup\$
    – Amy Fawcett
    Commented Sep 18, 2019 at 13:41

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.