Tiny PCBs - score, route, or ?

Express PCB has a board size minimum which i think exceeds what you want. BUT. They have this special price on a (roughly) 3x4 board, *and* they now (in their latest software) allow one to indicate routing... So... Layout one board in the upper left of the standard low-cost area, and then group, step and repeat them using 0.1 inch routing cuts (seems to be standard) and leave (say) 0.15 from center of cut to an edge, so that the worm-eaten board is still one board. A little strip of waste on the right and/or bottom is acceptable, because you may get a dozen units per board. Snap apart when you get them, and file the tabs. This is the least expensive way i know (yet) that small boards can be made.

I do not think the use of tin snips for cutting FR-4 should even be considered. Stresses the h*ll out of the board for a large distance, spreading a large distance from the cut itself.

:-) Ah, the voice of reason.

Yes, this is one of those negative-ROI projects, where personal interest overrides the soft costs. It's a niche product, so we might have to saturate that small market before we start to recover the true development costs.

A "huge" volume of these would require

Valid concerns, I'm sure. I expect it is also highly subjective to the rigidity of the joint (material, depth of groove / size of tabs) and the placement of the components.

It may be easy enough to test after separation instead, at least until the technique is proven under our specific conditions.

Thanks, Richard

(snip O/P)

Futurlec

depanelise free. I regularly order batches comprising 30 double-sided boards each 1.3" * 0.8" and the shipped cost is $US41.

Re the O/P, I appreciate he is concerned about stuffing tiny boards and appears to favour population before separation. I certainly prefer stuffing tiny boards in a small board holder rather than separating assembled boards from a panel.

So is it worth all your time and effort then to find the cheapest way to make them? Sounds to me like you have spent at least a day allready on it. What is your hourly rate?

--DF

The only routing I get from them is board outline - no slots or anything. But the results are very good/clean/straight edges and curves. I haven't used them for SMD, only through-hole.

Actually a job I sent them yesterday has slots - small ones for a DC power inlet receptacle. The Chinese fabs know what they are, and I guess in a couple of weeks I'll know how Futurlec handle them.

appears

boards

All my *small* boards have been through-hole. We had some ~2" * 2" SMD boards which we sent to a stuffing house that handles small batches (20). I really don't want to get into SMD stuffing, when there are firms that do it (even in Oz) for relative peanuts.

For the T-H boards the holder is a weighted base with adjustable "hands" that simply have a V-groove that clamps the board edge. Would be an issue if the board didn't have straight (and pref. parallel) sides ;-)

Depending what you are after, I note that Futurlec also do stuffing for >20 batches. Never had occasion to try it. Depending on the load this may also help. I try to stick to my "core business" and leave tasks such as board fab, SMD stuffing etc. to houses that have that as their core business.

If a board house is doing it, can't you ask them to just shear them? Or do you want them together for stuffing?

Thanks, Rich

Yes, that's the deal. It's a hell of a lot faster to assemble one big board with 200 parts manually than 20 boards with 10 parts each.

Best regards, Spehro Pefhany

--
"it\'s the network..."                          "The Journey is the reward"
speff@interlog.com             Info for manufacturers: http://www.trexon.com
Embedded software/hardware/analog  Info for designers:  http://www.speff.com

I have been using 0.032" thick scored FR4 panels of 100 boards per panel. Each board is 0.4" x 1.0" All components are surface mount. Top and bottom scoring must line up accurately for good depanelization. Traces run 0.025" from the score line. No sanding required.

Regards,

Boris Mohar

Got Knock? - see: Viatrack Printed Circuit Designs (among other things)

void _-void-_ in the obvious place

I have posted a PDF in alt.binaries.schematics.electronic of a tab layout I like to use. I make the tab a footprint so the board house won't make a silly choice. Position the tab away from resistors and capacitors as they are susceptable to cracking if they are too near the breakaway point. This tab works on 0.062" thick FR4. A quick brush on sandpaper will remove the jaggies if needed. You can reposition the drill holes to suit your needs.

This particular panel was run thru Circuit Express , a prototyping house, due to customer request. I normally use US Circuit for small to medium runs.

--
Mark

Got it - thanks! Real-world examples make great references.

I'm not following you on this one - what do you mean by footprint? Meaning you spec the routing pattern as a layer (which I'd plan to do)?

Makes sense. I'm planning to have PTH connectors closest to the edge, but how far back do you recommend keeping SMD from the snap? Is 0.03" enough?

Also great info. Neither of these were on my list of ~40 vendors to check with.

Thanks! Richard

Nice. Thanks for the specifics, Boris!

I hadn't thought about whether they'd align the scores on both sides (or for that matter, score both sides...)

Who do you use for your small boards? Do you find 0.032" is cheaper, or did you go that route for other reasons? We're pretty flexible in that regard.

So far, futurlec.com is coming in cheapest at $50 job + $0.65/square inch with full mask & screen, and scoring or depanelizing. At least now we're into the realm of "affordable" trial & error...

Thanks, Richard

Footprint is a PCB component. Thus, I make the drill pattern for the tab a PCB component and position it where it makes most sense, like away from parts. You'll notice that I have the tabs staggered to give the boards a bit more stability in the panel.

On 0.062" FR4, I would keep SMD resistors and capacitors at least

0.100" away from the drilled tabs. You might get by with 0.050". More is always better. You can also mess up thru hole plating if they are too close to the snap. I've had the most problems with 0402 SMT ceramic caps cracking near shear lines on thin (0.032") boards. Orienting the part parallel to the shear line is helpful as it puts less stress on the part.

US Circuit is a joy to work with. I've been using them for 12+ years.

I am using local supplier

who although twice as expensive provides unquestionable quality. At the quantities I make them (100s) the material cost is not so significant. 0.032 was a customer requirement.

Regards,

Boris Mohar

Got Knock? - see: Viatrack Printed Circuit Designs (among other things)

void _-void-_ in the obvious place

Got it. Creating a component makes a lot of sense for consistency and ease. I didn't notice the offset tabs at first, but that's a good technique to get away with fewer tabs.

Have you considered dropping the carrier strips and butting the boards up against each other? You'd have to add vertical tabs for rigidity, but it might yield another column per board. Or is board cost not enough to outweigh potential issues with assembly (flexing)?

(Our boards are about 1/4 your scale, so without carrier strips our yield would nearly double per board.)

Good to know. How was your experience with Circuit Express (cost, volume, quality)? It turns out they're local to us, which is appealing.

Thanks, Richard

We use Advanced Circuits, and despite our flaunted expertise :-) and our best efforts, they always seem to find a few issues in the pre-flight inspection of our submitted files. Generally we get perfect PCBs as a result, after a few day's delay for fixes.

--
 Thanks,
    - Win

I'll let you know when I've given it a try. For this item, I can't see volume ever justifying P&P setup, but I'd like to design to that goal and be ready when the next project needs it.

Good thought. I've never noticed it done that way (perhaps to its credit), but it seems viable - just a bit change in the router.

Thanks for the comments on Circuit Express. I've pinged them to see how creative / flexible we can get this.

Cheers, Richard

Hi, Win.

We've used Advanced Circuits as well, with excellent results - their work arrives exactly as expected. No surprises, which is about the best review I could give.

Unfortunately, their prices are "really high" - their magic number seems to be $500, which I can appreciate as a businessman, but not as a customer. In contrast, a shop in the $100 range encourages more experimentation, iterative improvements, and faster forward progress.

I think they're on the right track with their 33each.com service. It'd be nice to see its options expanded.

Cheers, Richard