8
\$\begingroup\$

What rules and tips make automated assembly easy, rather than unnecessarily difficult or completely impossible?

In particular, if I have a circuit board that works fine after hand assembly, some people imply that they may not be suitable for automated assembly:

"The prototype-type PCB fabrication places will send you printed circuit boards, ... These boards are suitable to test your circuit, ... They can be used for HAND ASSEMBLY of your circuit. They will generally not be suitable for an automated assembly process." -- Scott

What things are Scott referring to that I might need to change before going to mass-production automated assembly?

After telling me "Always do A, and never do Z", please go on. Why you do that? What problem(s) does it avoid? Is there a book or website that discusses design-for-assembly tips?

\$\endgroup\$
  • \$\begingroup\$ Perhaps what the answer means is that the manufactured PCB's themselves are not a suitable input to automated assembly. Automated assembly plants need control over the whole PCB process: the inputs have to be drawings, not ready-made boards. OK, imagine that you had a PCB made, but they did not drill any of the holes. Could you just hand the PCB's to another PCB plant and say, "drill the required holes in these?" Quite imaginably, even with a drill file, they would have difficulties and it would end up being done by hand. \$\endgroup\$ – Kaz May 25 '14 at 4:48
  • \$\begingroup\$ I was about to ask the same question. I just sent off a design to get a quote for PCBA. One of the SMT components has to be on the bottom of the board and apparently that is a bad thing. I wonder what other things to avoid. \$\endgroup\$ – geometrikal May 25 '14 at 6:45
  • 2
    \$\begingroup\$ Excellent answers so far, I also recommend watching this video and part 2. youtube.com/watch?v=VXE_dh38HjU \$\endgroup\$ – Matt Young May 25 '14 at 17:12
7
\$\begingroup\$

You'll typically want to panelize boards made for machine assembly. Loose boards are going to be more expensive to populate because special fixtures have to be manufactured and used (unless it's got really wide unused areas on the sides), and because there is more handling to populate (say) 12 single boards than a 4x3 panel.

That means more up-front NRE and tooling costs and more per-unit cost, which is pretty much the general result of not following guidelines.

You should put adequate tooling strips on the sides (typically 10mm bits that will be snapped off and discarded), tooling holes on the strips, and fiducial markings at least diagonally opposed on the tooling strips (for alignment), and diagonally about any high-density BGA footprints. You can see the fiducial marks (dots) on the tooling strips below.

enter image description here

Here is an example of using "mouse bites" and routed outline to allow such a PCB to be depanelized with a minimum of drama:

enter image description here

The board can be snapped along the lines with close-spaced (unplated) holes, leaving a smooth edge most of the way around. (the image shows a couple of ways of making the outline, but typically you'd need an additional routed line or V-groove to separate the boards in the other dimension). I prefer V-grooves alone to mouse bites for volume boards, but it tends to cost a bit more, and they must extend all the way across the panel, which can be limiting. You have to pay attention to the stiffness of the panelized board assembly or it can cause problems in the assembly operation (so you can't cut too much away on a thin board).

Sometimes you can put test coupons for controlled impedance, wiring to power boards for testing or other disposable circuits on the tooling strips.

You'll want to minimize the setups and operations. A relatively small number of different SMT (only) parts only on one side of the board with adequate spacing should be cheaper for machine assembly. Anything that cannot be supplied in a tape and reel with a proper leader will cost more to assemble.

Minimize the number of different parts on the board (there are only so many part feeders on a P&P machine- 25 to 40, perhaps). It may be better to use a few more of the same part or otherwise rationalize your use of parts (if you need a 4K7 resistor for an analog circuit, maybe pick that for all your pullups, if you are using a zillion 100nF/10V ceramic bypass capacitors, try to to use them in other locations.

Much more could be said, and the illustrious Australian Dave Jones has some good videos on the subject- he was a professional PCB designer and has worked for Altium, so they're quite good if you use Altium. (often you can get the link from the right sidebar in SE) Altium has good built-in tools for panelization but, of course, you have to know what dimensions you want to use for the panel, spacing, route widths, allowance and copper-pull-back around V-grooves, fiduciary marking dimensions etc.).

Some of this varies from manufacturer to manufacturer, but there is a lot of common ground. Don't make the panel too big to fit in the assembly machine(!), something around 9 x 12" or thereabouts is usually fine for modest size individual boards.

The board itself should have adequate spacing between the parts, preferably no parts hidden under other parts or on the bottom of the board, proper pad dimensions, and unplated holes where desirable. Slots should be used instead of huge holes if through-hole parts have flat leads (eg. barrel connectors). Hole sizes for through- hole parts must have adequate clearance to account for tolerances or they can't be reliably machine-stuffed. Bigger is better (up until the point where soldering is compromised). If you need to cover bits for wave soldering (so holes won't get filled in, or connector tabs covered with solder), you need an additional masking or taping step. Parts that require alignment (through-hole LEDs, for example) can require custom jigs or fixtures, for which you might have to make allowances on the PCB.

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

Basically you will need two consider three main issues here.

  1. Using the stencil to apply solder paste. This is usually a non-issue, but for specific parts (e.g. parts that require lots of solder paste (such as a connector for mechanical strength) or parts that have very small/thin pads. But if you were able to populate these parts per hand there shouldn't be an issue here.

  2. Placing components on the PCB: Usually the components are placed in vertical direction at 90° by the machine. A problem can arise if you have very small components next to large components. Usually the small parts will be populated first, then the large ones so it's usually not a big deal either. This is a task of the fabrication house since this may vary between machines. When you order the raw PCBs they will be delivered with a small border around them so the machine can handle it. If you have the PCB only without that border (which is removed afterwards) our machines cannot handle the PCB properly. You mention that "placing one part on the bottom is a bad thing". It is not, but the process will be more expensive since the boards will go through the machine and oven for a second time (or it is done be hand). Also, when there are "heavy" parts on both sides, it is possible that one part may fall off when the boards go through the oven a second time. Again, this can be worked around (some adhesive), but your product will be more expensive.

  3. Mounting through-hole parts: If you are not using a special technology such as Pin-In-Paste or similar, such parts may be placed by hand and the board will be soldered (again) even through wave soldering or selective soldering. Special rules may apply here (minimum distance, direction, ...)

Long story short: Every fabrication house should be able to send you their design guides/rules/documents up front so you will know what to look out for. And: The more complicated the layout, the more expensive it will get.

\$\endgroup\$
2
\$\begingroup\$

Mostly I was talking about the idea that you specify ONE board to a prototyping PCB printer, but you may need to pay attention to how multiple boards are panelized the production process. Runners must be added. If you have connectors that hang over edges, this may need some special though to make the boards easy to separate.

Also, there are imaging processes that are used to correctly position pick and place parts. Fiducials may need to be on your runners or on each board, or both.

This may or may not be an issue, as your fabricator may do some or all of this for you -- but the more you understand about the process, the better your conversations will go.

As to mixing SMD and through hole, that means two processes instead of one. Two sided boards are reflowed twice, and large pieces may need to be glued so they don't move on the second reflow. This adds cost.

As suggested in comments, I also meant that the boards you get from the prototyping PCB maker are already separated, and thus not suited for pick and place.

\$\endgroup\$
  • 1
    \$\begingroup\$ Thank you for filling in the details you alluded to earlier. \$\endgroup\$ – davidcary May 26 '14 at 3:17

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.