0
\$\begingroup\$

I am designing a board with the usual layer stackup of

Signal GND VCC Signal

On it I am placing a STM32F446VE which is 100 pin lqfp. As I am routing to every single pin on the package, and the pins are quite fine, the faning out of the pins is quite challenging.

To free up some space I toyed around with the idea of placing the many bypass capacitors on the other side of the board.

My first idea was to route it like this (a little tighter of course, this is just an example!):

enter image description here

This would ensure that all the current passes by the capacitor before it reaches the power pins on the processor.This however would not work as the vias connecting the capacitor to the processor are still part of the VDD and GND net and would therefor still internally connect to the power planes meaning some of the current would still pass through those vias directly and to the pins, not past the capacitor.

Is there a way in KiCad to ensure the vias would not connect to the inner power planes? Define the power planes around the vias?

I was not able to come up with anything simple, so some other routing ideas I had where the following. They still would not have all of the current past the capacitors but would be a little smaller IMO:

enter image description here

What is the proper way to route this? and does this matter? Also, are vias on pads like in the 2nd picture a problem?

\$\endgroup\$
4
  • 1
    \$\begingroup\$ "some of the current would still pass through those vias directly and to the pins, not past the capacitor" - Sounds like a misconception. You can connect supply lines to the chip any way you like; just make sure you also have a bypass connected to the pins not too far away. \$\endgroup\$
    – JimmyB
    Jul 22, 2016 at 13:12
  • \$\begingroup\$ Alright makes sense! \$\endgroup\$ Jul 22, 2016 at 13:15
  • \$\begingroup\$ 2nd picture is better because tracks between cap and chip are shorter. But via-in-pad can be a problem for manufacturing. If you solder manually, it doesn't really matter but if you use standard reflow process, you should avoid it. Place the via as close to the pad as possible, but not in it. \$\endgroup\$
    – dim
    Jul 22, 2016 at 13:19
  • \$\begingroup\$ Note that 'not too far away' is a subject in its own right, but provided you do not have outputs that transition in less than 200 ps (they definitely exist), then placing bypass on the opposite side of the board as shown is fine. \$\endgroup\$ Jul 22, 2016 at 13:25

1 Answer 1

1
\$\begingroup\$

I don't see any real problems with your first option. Is it ideal? No. Will it work fine for the part in question? Yes.

That the vias are connected to the planes aren't a problem, you are still providing a local source of power very close to the pins, that's the primary requirement.

If something like that was a problem then it would be virtually impossible to bypass a BGA package.

As already mentioned the via in pad can cause problems. Some PCB manufacturers won't like it and if you use a reflow process to assemble the board there is the problem of solder wicking through the via leaving a dry joint.

\$\endgroup\$
1
  • \$\begingroup\$ Via in pad in my experience means the vias are filled with some kind of epoxy to prevent solder wicking into them. If it weren't for this added step, there'd be no reason for the PCB manufacturer to care that you had via in pad. The assembly shop, of course wants the in-pad vias both filled and plated over (via-in-pad plated-over or VIPPO) to provide good yield in reflow assembly. \$\endgroup\$
    – The Photon
    Jul 22, 2016 at 15:46

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.