4
\$\begingroup\$

I usually work with big components (0805, 0603.) Now I'm trying to make a board that would use much smaller packages such as 0402 and 0201.

I know that balancing copper is relatively important to avoid tombstoning. How do I know if mismatches are tolerable or not? I couldn't find any clear enough information about this subject online, so here I am.

For example, I have this capacitor:

Capacitor test 1

In this case, I have 3x 8 mil for GND and 2x 8 mil for BAT.

Same in this situation:

Test 2

Here I have 3 capacitors with a basic copper balance. It seems that there is a lower thermal conductance between ground plane and the middle one than between ground plane and the side ones. How can I be sure that this difference is acceptable?

\$\endgroup\$

3 Answers 3

Reset to default
7
\$\begingroup\$

From my experience, your copper is very well balanced. The IPC has something to say about copper balancing:

enter image description here

\$\endgroup\$
5
  • 1
    \$\begingroup\$ According to the chart, his second picture matches the second row for IEA 0402 which says "Acceptable NOT Recommended". Am I reading the chart right? \$\endgroup\$
    – Rodo
    Commented Oct 16, 2023 at 17:04
  • \$\begingroup\$ The paths on the second picture don't all go to a larger copper area, though. Assuming it's about net heat flux away from the solder joint, and assuming it's reflow so everything gets heated at once, the paths between two components should be less impactful. \$\endgroup\$
    – Glenn Willen
    Commented Oct 16, 2023 at 20:10
  • \$\begingroup\$ @Rodo you are right, this is an edge case. But because the track width on the lower side is rather big I don't expect problems. And it's still "Acceptable" ;) No need to make the job of your manufacturer too easy :D \$\endgroup\$
    – jwsc
    Commented Oct 17, 2023 at 5:32
  • \$\begingroup\$ Alright, thank you for you insight and the IPC extract, it reassure me as my manufacturer was really emphasising the importance of copper balance in our discussion \$\endgroup\$
    – BEN
    Commented Oct 17, 2023 at 8:33
  • \$\begingroup\$ Could you provide the source of this image? \$\endgroup\$
    – asdfex
    Commented Oct 17, 2023 at 9:56
2
\$\begingroup\$

Your copper distribution should be fine from my experience. When in doubt, you could (and should) always asked your CM. Your CM can also give you land patterns that work fine. Often times it's the land pattern that causes tomb-stoning and not copper distribution.

\$\endgroup\$
1
  • \$\begingroup\$ Thank you, I'll check with them what info they can provide \$\endgroup\$
    – BEN
    Commented Oct 17, 2023 at 8:34
0
\$\begingroup\$

It's not only about tomb-stoning, it's also about drifting (unwanted rotation of the components during flow soldering).

In the first picture the component will drift north, but in this case, the sides will drift evenly so it won't be that bad. You can still avoid that by adding a forth trace to GND and a third one for BAT or joining the two traces on opposite sides of the pad, at equal distance from the center of the pad. Do this only of you correct the two pads. If you correct only one pad, it could be worse as it may drift non evenly.

On the second picture, add a third trace on the first 2GND pad from the left, symmetrically opposite to the trace on the third pad on the right. Try to make the trace going to 1NS21 and VDDBUCK straight (for 1mm or as long as you can) before going oblique.

Everything is about symmetry.

\$\endgroup\$

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