I'm designing a SMPS PCB with a pretty high current goal (using it to power multiple servos.) Using KiCAD, I decided to use solid fills on the pads of the high current areas, but by default thermal reliefs are enabled. This takes the large filled zone and necks it down to small areas.

I've read that with the right size soldering iron, this is no problem, but I was thinking of paying a little extra and just having the PCB fabricator assemble the board to save myself from SMD soldering, and then I can shrink some of the components.

Would a typical hobby/prototype PCB fabricator balk at having to assemble boards with solid filled zones connected to the pads?

KiCAD Screenshot

Edit: I maybe wasn't clear enough, I am not concerned about hand soldering these large packages. I have other components that are much smaller, like 0603 and TSSOP packages, the board also has components on two sides. Instead of trying to solder it myself, I was thinking of paying the PCB fab house to assemble the components as well. My question is will solid filled zones on these high current large traces affect the PCB assembly house if designed like in the second picture below. Will the components float/not align properly, or does the silkscreen alleviate that?

Filled Pads

  • \$\begingroup\$ if you want to solder these by hand you could rotate the capacitor footprint 90 degrees, and have thin traces. electrolytic capacitors have fairly high ESR compared to copper traces. \$\endgroup\$ Commented Jun 29, 2018 at 6:32
  • \$\begingroup\$ Those traces are far away from a size too big to solder by hand \$\endgroup\$
    – PlasmaHH
    Commented Jun 29, 2018 at 6:40

3 Answers 3


For SMT/SMD technology, solid filled pads are no problem, if you use a reflow oven that heats the whole PCB up to the melting point of the solder joints. This reflow oven can be as simple as a small pizza oven (That’s what I use at home for reflow soldering).

But if you try to solder solid filled pads with a solder iron by hand, this can be tricky.

Edit1: So your Pcb fab will have no problem when soldering pads embedded in large traces, because they mostly use a reflow oven.

If you design the traces symmetrical (i.e. both sides of the pad have same trace widths, there will not be a floating/aligning problem, too.

  • \$\begingroup\$ How hard it is to solder by hand is of course depending on the line which is connected. If you are trying to solder something to ground on a board which has a dedicated ground plane all over, yes the heat distribution will make it hard since you are heating the entire plane. If it is just a signal connection on a top of bottom layer this will be much easier to do by hand. \$\endgroup\$
    – Remco Vink
    Commented Jun 29, 2018 at 6:35
  • \$\begingroup\$ Thanks for the answer, I updated my question. I am unclear if a pcb assembly house would have difficulty assembling SMD components with solid filled zones on large traces, not if I can hand solder them. \$\endgroup\$ Commented Jun 29, 2018 at 16:05

There should be no problem with the PCB fab house.

This is how the pad could be done.

Use 2 extra pads to provide solder mask and 2 more to give you a copper pad.

Pad 1 is the existing pad with only F.paste and F.mask checked.
Pads 2 and 3 all "technical layers" are unchecked.
Pads 4 and 5 only has F.mask checked.

Pads are numbered for explanation, renumber them all to the original pad number.

enter image description here

The two green pads (2 & 3) are the solder resist.
The two end pads (4 & 5) are copper, where you can heat the solder if you do not want to use an oven.
The solder resist pads (2 & 3) could / should be narrower.

enter image description here

You can buy SMD solder paste in a syringe.
Apply solder and drop components
Apply heat with iron.

enter image description here

To use the oven

  1. Heat the oven to 500°F.
  2. Put the PCB in the oven
  3. Turn off the oven.
  4. Wait 90-120 sec.
  5. Remove from oven

Soldering 0603 to a large copper area with a proper reflow oven or a hot air rework tool isn't that hard to do, although some people might have concerns about your board yield if attach one side of the board to a large copper area, and the other side to a thin trace. Just look up tombstoning.




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.