22
\$\begingroup\$

I am attempting to replace an old PLCC32 part that was directly soldered to the board with a new part of undecided form. We will definitely need an adapter as we have not been able to find a PLCC32 part that does what we need. I cannot use a PLCC adapter plug because there are also height restrictions. We are considering building a two-sided adapter board that has pads on the bottom side that match the PLCC32 layout on the current board, with the new layout on top. Theoretically, the adapter board would be soldered directly to the old board and the new chip on top of the adapter.

However, I have not seen any examples of soldering two PCBs directly together in this manner, which makes me think it is a likely to be a bad idea. Can anyone comment on this sort of custom adapter?

\$\endgroup\$
23
\$\begingroup\$

No problem. I had to look for a picture that illustrates the technique:

enter image description here

You make a PCB with plated through holes on the PLCC's pads, so at a 1.27 mm pitch, and mill the four sides so that you get the half holes like in the picture. These are easily solderable on the old PLCC footprint, it's an often used technique, called castellation.

A picture of a complete board:

enter image description here

and another one:

enter image description here

or this one from a question posted 1 minute ago:

enter image description here

You get the idea.

You'll have to find a part which fits inside this small PCB, but given the miniaturization of the last years that may not be a problem.

edit 2012-07-15
QuestionMan suggested to make the PCB a bit larger so that the PLCC's solder pads are under it. For BGAs the solder balls are also under the IC, but that's solid solder balls, not paste, and I don't know how solder paste will behave when squeezed between two PCBs. But today I bumped into this IC package:

enter image description here

It's the "Staggered Dual-row MicroLeadFrame® Package (MLF)" of the ATMega8HVD, and it has pins under the IC as well. This is 3.5 mm x 6.5 mm, and weighs a lot less than the small PCB. That may be important, because thanks to the low weight capillary forces of the molten solder paste can pull the IC to its exact position. I'm not sure if that will also be the case for that PCB, and then positioning may be a problem.

\$\endgroup\$
  • \$\begingroup\$ Can you comment on any specific instructions to the board house for the 'half pads' along the edge? It must be significantly different from the plated through hole process. I can't think of how I would even represent this in my ECAD (Altium). \$\endgroup\$ – Jason Jul 12 '12 at 17:21
  • 3
    \$\begingroup\$ @Jason - I think that you draw them like any regular hole on a PCB which is a bit larger, and pass an outline drawing which cuts the holes in half to the PCB shop. You'll have to instruct the DRC to ignore that the holes are overlapping the PCB's edge. Milling of course, no V-cut :-). I don't know if the plating is something special. \$\endgroup\$ – stevenvh Jul 12 '12 at 17:25
  • \$\begingroup\$ What about expanding over the original chip layout with SMD pads, e.g. without the castellations? SMD pads on the bottom so the top layout can be larger than the original pads. \$\endgroup\$ – QuestionMan Jul 12 '12 at 18:19
  • \$\begingroup\$ @QuestionMan - I don't know if they do this with reflow solder paste. BGAs use this technique, since the BGA carrier is actually a thin PCB, but then you would have to find some solder balls and a way to attach them. Also a well controlled reflow oven. \$\endgroup\$ – stevenvh Jul 12 '12 at 18:27
  • \$\begingroup\$ @stevenvh I asked my board house about this and they basically confirmed what you have said (outline through holes and inform in fab notes). Their term for this is 'half holes'. \$\endgroup\$ – Jason Jul 12 '12 at 19:15
8
\$\begingroup\$

Soldering a small PCB flat onto a larger PCB is possible. In fact, that's how many of the embedded radio models are mounted (example, example). The pad can be on the edge of the board (via cut to form a half-cylinder*). Or, the SMT pads are either directly underneath.

* see also photo in stevenh's answer. Such feature is called castellation (thanks, The Photon).

Look also at Aries Correct-a-Chip adapters. Some of them (like this one) go from one SMT footprint to another SMT. There are also companies that specialize in making custom adapters. adapters-Plus, for example.

\$\endgroup\$
  • 4
    \$\begingroup\$ "castellation"? \$\endgroup\$ – The Photon Jul 12 '12 at 17:23
  • \$\begingroup\$ @ThePhoton "castellation" Yes, that's it, thank you! \$\endgroup\$ – Nick Alexeev Jul 12 '12 at 17:37
  • \$\begingroup\$ @ThePhoton - You could have said that sooner!! I've tried about every possible keyword on images.google.com!! Dammit ;-) \$\endgroup\$ – stevenvh Jul 12 '12 at 17:37
  • \$\begingroup\$ Almos all your links are dead. \$\endgroup\$ – Navin May 11 at 6:21
7
\$\begingroup\$

They make adapters for just about every footprint to any other footprint. And if it's not made, there are companies that will make one custom for you. But they are usually pretty expensive and, as you mentioned, tall.

enter image description here

Another option is deadbugging the chip. But looking at your other question, you have a production run of ~70K units. So this solution would seem impractical. The chances of a wire being placed incorrectly or a solder joint not holding (especially if subjected to vibration) are probably too great on a run that size. And when you factor in technician time, it is also pretty expensive.

enter image description here

They do make BGA adapters so something that is more solid than deadbugging and shorter than a normal adapter is possible. In order to accept another PLCC32, the board would proabbyl need to be bigger than the original PLCC32 footprint and soldered using solder paste on the original pads and a reflow oven like a BGA component would be. Then the new PLCC32 would be soldered on the adapter's pads. Again, expensive.

enter image description here

Your best bet would be to consider using a new chip with a smaller footprint. Then having a small board made up that is the size of a PLCC32 with similar pins. I've seen something similar for 8051 ICEs. I couldn't find a good picture though.

For a production run of the size you're talking about. I would at least price out respinning the board. Comparing to the cost of a custom adapter plus technician time to install, the respin may be cheaper in the long run.

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

I'd consider a Ball Grid Array (BGA) IC package to be close to an example of that. It comes with solder-balls preplaced on the "component" PCB. Assembly is tricky, usually done via automated placement and hot air, frequently with preheat from below too. In your case you presumably would only have contacts around the periphery so inspection would be a bit easier. However you probably won't have the preformed solder balls. You might look at rework solutions for re-balling BGAs.

There is also some similarity to a QFN package, which is usually soldered by depositing paste with a stencil and then using a similar external area heat source, however you won't have the metalization up the edge thickness which many QFN's have to aid filleting (and incidentally give you a limited ability to do rework with an extremely fine-tip iron)

If your PCB house will do it, the plated through holes cut in half by the board outline idea seen on some recent chip-carrier modules might be an interesting idea, as that would give you metalization up the thickness. I think you might have a fair shot of soldering that on with an iron or an air pencil.

\$\endgroup\$

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.