12
\$\begingroup\$

I'm designing two boards that'll always be used together. I'd like to place them both on a panel and break them apart after manufacturing.

I found a document on PCB CAD Design Guidelines that explains breakaway tabs and lists guidelines for their design.

Board assemblies can be de-tabbed using perforated breakaway tabs, v-grooves breakaway tabs, or hand-cutting with a de-tabbing tool.

However, how would I indicate break away tabs in the CAD file? For the perforated tabs, I could add through-holes in a line (although I hope there's a more standardized method), but I'm not sure how to indicate v-grooves.

Also, what concerns should I be aware of with breakaway tabs?

\$\endgroup\$
  • \$\begingroup\$ I've sent mechanical-style drawings of the PCB arrays to the fab along with the gerbers. My drawings didn't have breakaway tabs. The fab added tabs and sent me panelized drawings, which I've approved. Don't know if every fab would work this way, though. Also, here's an article from PCB Design & Fab magazine The PCB Array, and Why We Use It. It also mentions breakaway tabs. \$\endgroup\$ – Nick Alexeev Jul 20 '12 at 23:15
8
\$\begingroup\$

I'm sure that processes vary from place to place, but it's been my experience so far that when a PCB needs to be panelized, two drawings are generated:

  • a standalone file, and
  • a panelization or array drawing.

The standalone file is the usual PCB drawing, showing the etching, vias, dimensions, etc. for the standalone PCB. There's no graphical indication on this drawing that the PCB is part of a panel.

The panelization drawing shows how many of the individual PCBs are to be included on a single panel by showing multiple standalone PCB outlines, along with the details of how they're joined (v-groove, breakaway tabs, etc.) - the specific PCB details other than the outlines (and any slots/holes therein) are omitted from this drawing.

For example:

panelization drawing excerpt

This excerpt uses breakaway tabs and v-grooves.

You generally need to keep components away from any depanelization areas, as the mechanical stress of depanelization can sometimes inflict some mechanical stress on nearby parts (ceramic capacitors can crack, for instance) - the tool that's used (v-groove cutting wheel) may need some clearance as well. You wouldn't want filet-o-capacitor on your finished goods.

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

You can either choose panelization drawing or let Fab shop do it for you. It only takes seconds. What you need to do is define the method of breakaway on a drawing in text . Such as V-score with no protruding edges or corners or milled with 3 micro-via holes on breakaway tab. Ask your wave-soldering engineer to review fro flex issues since glass transition temperature weakens the panel and flux leakage over solder wave can create a fire hazard if board dips into solder.

Consult with vendor for best method for them . Beware if your de-panelization method applies too much stress to boards post SMT solder, big ceramic chips can crack. So get Process Eng. to review for stress on rapid de-panelization method and training required.

Many simple solutions for panelization can be overlooked in the design that cause defects later.

Structural strength of panel at room temp is significantly weaker at oven or wave solder temps, so twist warp is a major factor to consider in aspect ratio and size of panel, in addition to depth of V-score and ease of breaking. Major tradeoffs

Drawing is simply an outline and details in words, unless you have complex non-rectangular shapes where milled outline works better or triangular break shapes..

\$\endgroup\$
0
\$\begingroup\$

There is no really standard way to do V-scoring.

Easiest solution would be just adding silk screen at that place and writing a separate instruction for manufacturers.

E.g. 4-PCB

\$\endgroup\$
0
\$\begingroup\$

That is a question that you should ask to to the PCB manufacturer you will work with since that may vary from manufacturer to manufacturer.

But according to my experience, it should be easier than you think.

The manufacturer I work with only requires that the boards are in a panel respecting the spacing between the boards they specify (in my case I use 2.5mm but it can vary for other manufacturers), the manufacturer takes care of the rest, I never had give specific instructions for panels never had a problem.

I'm using eagle and I'm specifying the board contours on the dimension layer.

Some manufacturers have these instructions on their websites.

\$\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.