I have a question about PCB copper planes with buck converters. For reference, I'm using the LM2673/LM2679. The parts are identical in layout, utilizing the DDPAK/TO-263-7 with the PCB tab being connected to the IC's ground pin (pin 4).

Initially, I'm laying out the device on a 2-layer board with the top plane consisting of signal traces only (so you have isolated copper planes on top alongside the traces), and the bottom plane being the ground. However, seeing as how the tab is connected to ground, it seemed more convenient if both planes were ground planes for both the SMT components as well as for thermal dissipation. If I were to use ground pours on both sides, what are some areas which are recommended to keep copper fills out?

EDIT: I found this TI thread that kind of delves into what I'm talking about. I'm using shielded inductors, and based on what it's saying, it seems to promote the idea of removing the top layer copper under the inductor (while keeping the bottom copper filled) in order to avoid EMI issues. So, even though my inductors are shielded, it seems to be better practice if I keep the area of the inductor free from copper. I was wondering if I should apply this practice to other components as well.


  • \$\begingroup\$ Why do you need copper fills out? \$\endgroup\$ Jun 2, 2020 at 17:43
  • \$\begingroup\$ @VladimirCravero I think OP just knows that there are some situtations where copper fills are bad but isn't sure what these situations are. I am not aware of any situtations where they are bad for something like a buck converter where you're not impedance matching anything. Don't leave copper pours floating though. \$\endgroup\$
    – DKNguyen
    Jun 2, 2020 at 18:12
  • \$\begingroup\$ @VladimirCravero I saw some recommended layouts where the switching inductor did not have copper underneath in order to reduce EMI or something like that. I don't exactly know the reason why. electronics.stackexchange.com/questions/452922/… \$\endgroup\$ Jun 2, 2020 at 18:23
  • \$\begingroup\$ @DKNguyen Thanks for your reply. I've seen many examples of layouts where, for example, the space underneath the switching inductor has no copper underneath in an effort to reduce EMI or something like that. What do you mean exactly by not leaving copper pours floating? If the top plane is designated as 'no signal', then you got floating copper islands, but do you mean they should be tied to something? rohmfs.rohm.com/en/products/databook/applinote/ic/power/… \$\endgroup\$ Jun 2, 2020 at 18:26
  • \$\begingroup\$ @user101402 Yeah, they should be tied to GND (or something). Don't leave them floating. I looked up why no copper under inductor and it's to prevent the inductor from inducting eddy currents in the ground plane. I only spent two minutes looking but found nothing definitive about how bad the effect really is. If the inductor is shielded it apparently doesn't matter much. \$\endgroup\$
    – DKNguyen
    Jun 2, 2020 at 18:38

1 Answer 1


regarding magnetic circuits, the placing of copper directly under the inductor is the same as providing a SHORTED_TURN near the inductor but with AIR as a key part of the magnetic path.

Given the top copper could be 1mm or even closer to portions of the inductor flux, the shorted_turn phenomena is strongly dependent upon the inductor/core/mounting_pins mechanical design, and thus is unpredictable.

So just remove top_layer copper under the inductor.


For any guidance on removing BOTH layers of copper under the Inductor, I'd call up the Reference Design designer/EMI evaluation person.

Or call CoilCraft or a Ferrite manufacturer.

Again, the air_path (air + FR_4) and the fringing of flux outside the inductor are what we are considering here.

Without exact field descriptions, and PCB foil eddy current descriptions, we don't know the

  • 1) EMI

  • 2) losses (in-efficiency of the switcher) due to eddy current loss


Do notice the reciprocity of metal antennas and holes_in_metal_plates.

Both the metal_as_wire and the metal_as_hole will RADIATE EMI.

You don't want to provide an antenna.

Thus removing the bottom_layer copper UNDER the inductor, with that hole becoming an antenna, is not a good idea.

Making a slot_antenna, albeit not resonant, is not good EMI practice.

Notice ANY cutting of the bottom plane, under the inductor, is equivalent to providing a slot_antenna_radiator. Currents will circulate around the edge of the hole/gap/slot, and even though a near_field antenna, bad things happen to EMI.

  • \$\begingroup\$ Thanks for your reply. That's what I seemed to be understanding based on my readings, so I decided to play it safe and remove copper pour directly under my inductor. I only removed it on the same plane as my inductor, so the copper pour on the opposite side of my board should be okay, right? Or is it common practice to remove that as well? \$\endgroup\$ Jun 3, 2020 at 14:13
  • \$\begingroup\$ @user101402 From what analog is saying, you should leave the far plane intact because cutting through all the layers makes a slot antenna which you don't want. \$\endgroup\$
    – DKNguyen
    Jun 5, 2020 at 3:32

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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