7
\$\begingroup\$

I just learned from the websites of a couple of board manufacturers that they can go as low as 0.8mm on a 4-layer board.

I think going to 1.0 mm (instead of my standard use of 1.6 mm) would be helpful since I am trying to optimize on space. Since there is a high density of traces, it would be desirable to have the convenience of the additional 2 layers during signal routing.

However, due to lack of experience with having 4-layer boards manufactured, I am concerned that issues may come up with a 4-layer board at such low thickness, e.g., problems with blind/buried vias, longterm robustness of the board, problems during pick-and-place assembly, etc.

For my final manufacturing, should I play it safe by sticking with the 1.6 mm thickness?

Or is board-manufacturing sufficiently reliable that I can expect the 1.0 mm 4-layer board to have no issues -- is it common in the industry to go to such low thickness?

UPDATE:

Details of PCB (as requested below):

  • 50 mm X 50 mm
  • Two Micro-USB connectors present (into which of course USB cables will be inserted/removed)
  • PCB secured into groove-type slots within plastic enclosure
  • No long/thin components: Only standard ICs, e.g., QFP-48 microcontroller, voltage regulator, etc.
  • One "heavy" component: A small OLED display panel is inserted into the 10-pin female headers located on the PCB.
\$\endgroup\$
5
\$\begingroup\$

You won't experience problems with vias: 8 or 10 layer boards 1.6 mm thick are common, and then the individual layers are thinner than a 4 layer board of 1.0 mm thickness.
A 1.0 mm PCB will be less stiff than a 1.6 mm, but unless you want to place a heavy transformer on it (don't!) this won't be a problem either.
Standard thickness panels may be up to 635 mm (25 inch) wide, but your manufacturer will limit that for 1.0 mm thickness. Ask him how wide a panel may be.

Overall, a 1.0 mm board is a bit less stiff, but for boards up to Eurocard format (160 mm x 100 mm) I wouldn't worry about it.

\$\endgroup\$
3
\$\begingroup\$

See also What are the advantages and disadvantages of thinner PCB thickness (<1.6 mm or 0.063'')?

My PCB manufacturer rep was showing off some 0.5mm PCBs recently. The panel was distinctly floppy, but the individual boards were coin-sized and apparently worked fine.

This is the main limitation, and is hard to answer either way without considering the mechanical design surrounding the PCB. Is force applied to the PCB? (connectors, switches) How large is it? Does it have mechanical support once in its casework? Are there any long thin components on it that will cause problems if it flexes?

\$\endgroup\$
  • \$\begingroup\$ Thanks for that reference. I also updated the question by adding the information you suggested I provide. \$\endgroup\$ – boardbite Oct 3 '13 at 13:56
3
\$\begingroup\$

Depends on your components. I have made a 0.8mm thick 4 layers FR4 board with QFN components and 0201 passives. There were issues with two big components (Broken solder joints) due to the PCB plate flexing during automated tests. The manufacturer solved it with glue.

\$\endgroup\$
  • \$\begingroup\$ What were the big components, or how big were they? \$\endgroup\$ – boardbite Oct 3 '13 at 15:20
  • \$\begingroup\$ Chip antenna (16mm by 3) and a mechanical motion sensor (SQ-SEN-200) \$\endgroup\$ – Lior Bilia Oct 3 '13 at 18:21

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.