3
\$\begingroup\$

I'm wondering if it's possible to place a through-hole connection on the opposite side of an SMT microcontroller.

I have a small connector with a solder pin (for the shield) on one side of the board, and I'm hoping to place a microcontroller on the other side of the board. The hole for the connector would be near the center of the MCU package, away from the pins.

The board is extremely space constrained and this might be the only way to get the MCU on the board without going to a tiny-pitch WLCSP type package. The position of the connector cannot move.

Has anyone done this? What are the challenges and things to keep in mind?

\$\endgroup\$
5
  • 4
    \$\begingroup\$ possible to place a throughole connection on the opposite side - thru-hole is by definition on both sides. \$\endgroup\$
    – Eugene Sh.
    Aug 22, 2017 at 18:25
  • 3
    \$\begingroup\$ The throughhole lead would need to be short enough or cut to keep from protruding on the other side. I'm worried about mechanical issues, or solder coming through the hole and causing trouble. \$\endgroup\$
    – sgdsgyhetwaraw
    Aug 22, 2017 at 18:30
  • \$\begingroup\$ As long as they do not interfere with each other mechanically, electrically, or thermally, then yes you can. \$\endgroup\$
    – Trevor_G
    Aug 22, 2017 at 18:30
  • 1
    \$\begingroup\$ Placing a TH lead under an SMD component is liable to be "problematic", as others have said. But you can more easily place small enough SMD components within the footprint of a TH components - subject to Trevor's constraints of non interference. SO it may be possible to move some passive or small active components under the connector so that the uC can be located elsewhere. \$\endgroup\$
    – Russell McMahon ♦
    Aug 23, 2017 at 11:07
  • 1
    \$\begingroup\$ If an SMD version of the connector does not exist it MAY be possible to trim the connector leads somewhat and surface mount it. This would place mechanical loading on the solder joints and the copper to substrate bond, and it would be 'extremely wise' [tm] to add mechanical strain relief in some manner - screws / clamp / adhesive / ... . If this is for one or a very few PCBAs this MAY be acceptable BUT it would be far better and far less risky to find a "proper" way to do this. \$\endgroup\$
    – Russell McMahon ♦
    Aug 23, 2017 at 11:11

4 Answers 4

Reset to default
18
\$\begingroup\$

The hole for the connector would be near the center of the MCU package, away from the pins.

This is a very bad idea.

Usually the pins from through-hole parts stick through the board by at least a millimeter, more than enough to interfere with the ability to place a chip where it would cover the pin.

You could conceivably cut the pin short enough that it doesn't stick through the board, but that's going to be a special operation and add cost. You wouldn't be able to inspect the solder joint with the through-hole pin because it would be all hidden in the hole.

It will also mean the chip has to be hand soldered because it has to be attached after the wave solder step is done to solder the through hole part.

If you had to rework the through-hole part, you'd have to remove the chip, rework the through-hole, and then re-attach the chip.

\$\endgroup\$
6
\$\begingroup\$

If it's a connector that you buy, the lead will definitely be longer than the board is thick, and this simply won't work out. Get an surface mount connector, or place either your connector or your microcontroller elsewhere.

\$\endgroup\$
4
\$\begingroup\$

I would recommend against this for the same reasons that @ThePhoton describes.

Is it possible to bend the shield pin and then solder it to the connector-side of the board? This extra step will cost you when you go into production, but not as much as all the custom assembly work that would be required with a thru-hole.

\$\endgroup\$
1
  • 3
    \$\begingroup\$ There may even already a surface mount version of the connector. Though one does need to beware of them ripping off the board and taking the surface foil with them - staking down with vias can help, but it makes a more delicate assembly, especially if it's likely to often be re-plugged. \$\endgroup\$
    – Chris Stratton
    Aug 22, 2017 at 18:45
2
\$\begingroup\$

I'm wondering if it's possible to place a through-hole connection on the opposite side of an SMT microcontroller.

I advise against that. The through hole leads will protrude through the other side of the board and keep the SMT component from seating properly.

I have designed circuit boards where SMT components nestle inside the legs of through hole components, but this is the opposite of what you asked.

Consider going to an SMT version of the connector, or possibly go with a through hole version of the micro, as through hole components have some margin for height adjustments off the board.

Another option: place the micro elsewhere and place other SMT components around the connector.

Also, consider going to a 4 layer board. Those boards allow you to push your power and ground traces onto internal plane layers, which frees a lot of space for component placement. You are looking at about a 20% increase in PCB cost. As a bonus, having internal plane layers provides (electrical) noise isolation, and you can do things like setup transmission lines for USB connectors.

\$\endgroup\$

Your Answer

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

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