Connect with us

Tiny PCBs - score, route, or ?

Discussion in 'Electronic Design' started by Richard H., Dec 28, 2005.

Scroll to continue with content
  1. budgie

    budgie Guest

    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.
    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.
  2. Richard H.

    Richard H. Guest

    Well, I have to give kudos to Futurlec - I dropped them a note and
    already got a reply. They will do v-scoring instead of separation, at
    no additional charge. That looks like a winner - thanks!

    Yep. One of the reasons I'm looking at panelizing - trying to work
    through a process that'll be easier to farm out when the volume supports it.

  3. Robert Baer

    Robert Baer Guest

    Express PCB has a board size minimum which i think exceeds what you want.
    They have this special price on a (roughly) 3x4 board, *and* they now
    (in their latest software) allow one to indicate routing...
    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
  4. Robert Baer

    Robert Baer Guest

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

    Populating, testing then snapping sounds to me like a way to introduce
    failures. I havent done it that way before, but from cutting and
    snapping PCBs unpopulated and populated, I'd be a bit surprised if you
    got away with it without causing failures. No doubt some here have done
    it and will know.

  6. Deefoo

    Deefoo Guest

    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?

  7. Richard H.

    Richard H. Guest

    :) 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 <12 medium-sized boards a year.
    At proto-house volume, the difference between shops is as much as 5x,
    which hugely affects the cost of goods and viability of the product.

    So, out of personal interest, it's worth sinking my time to drive down
    the hard cost of goods and see if a viable product can be turned out.

    Thanks for the thoughts!

  8. Richard H.

    Richard H. Guest

    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.

  9. Rich Grise

    Rich Grise Guest

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

  10. qrk

    qrk Guest

    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.
  11. 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
  12. Boris Mohar

    Boris Mohar Guest

    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.


    Boris Mohar

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

    void _-void-_ in the obvious place
  13. Richard H.

    Richard H. Guest

    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"

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

  14. Richard H.

    Richard H. Guest

    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

    So far, 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...

  15. qrk

    qrk Guest

    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.
  16. Boris Mohar

    Boris Mohar Guest

    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


    Boris Mohar

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

    void _-void-_ in the obvious place
  17. Richard H.

    Richard H. Guest

    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.

  18. qrk

    qrk Guest

    I was contemplating getting rid of the vertical carrier strip, but was
    unsure how flimsy the panel would be. The panels I make usually go
    thru pick & place machines. If your assembling the first lot by hand,
    I would try the panel without the carrier strip and see how rigid the
    panel is.

    I've also contemplated v-scoring the tabs. That would give you a very
    clean break. Next time I do a panel, I'll ask the board house what
    they think about that.

    I've only dealt with Circuit Express at arms length (customer dealt
    with them). They only do prototype or small quantities. They don't do
    production runs unless your production run is small. I've done cost
    comparisons with Circuit Express and US Circuit - US Circuit was
    slightly cheaper for a 1 week turn. That might have been due to the
    relationship we have with US Circuit (they know what to expect from
    us). The quality of Circuit Express is very good. I've seen sample
    boards from their roving salesman and a few of my customer's boards.
    Circuit Express appears to have very good pre-flight personnel. They
    caught a few questionable things on my boards that knowledgable folks
    would catch.
  19. Richard H.

    Richard H. Guest

    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.

  20. qrk wrote...
    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.
Ask a Question
Want to reply to this thread or ask your own question?
You'll need to choose a username for the site, which only take a couple of moments (here). After that, you can post your question and our members will help you out.
Electronics Point Logo
Continue to site
Quote of the day