Connect with us

How would you mount this package?

Discussion in 'CAD' started by Nathan Bialke, Apr 2, 2007.

Scroll to continue with content
  1. Hello,

    A magnetometer part I'd like to use - the Honeywell HMC1051Z - is only
    available in a 8-pin 50 mil pitch SIP package that I've never seen
    before. The datasheet is available at http://www.ssec.honeywell.com/magnetic/datasheets/hmc1052.pdf
    .. The pins are too large for me to fit into plated holes if I use
    "reasonable" design rules (20 mil hole with a 15 mil past the hole
    annular ring). I asked a technician who suggested surface-mounting by
    bending the pins into an "L" and then soldering the parts onto 50 mil
    pitch pads. However, I would rather find a better solution - it seems
    to me that the first time I brush the part on the board accidentally,
    I'll rip up the pads!

    Does anyone know of a way to mount this part that fits "reasonable"
    design rules and has some aspect of structural support?

    Thank you!

    - Nathan
     
  2. Nathan,
    That package certainly is a bit of an enigma.

    The only other suggestion I could make is soldering the leads flat to
    traces/pads with the body hanging off the edge of the board or within a
    cutout segment of the PCB.

    The leads seem to be a little short to offset them into two through hole
    rows, at least not without great care or a good jig to support the leads and
    not stress the package. It could work but care should be taken and I
    wouldn't want to do it for any number of devices without a proper jig.

    If you did "L" lead them ont SMT pads, bend each leg alternately
    (left/right, forward/back), that would help with overall support and
    integrity. Then you would also want to use silicon or epoxy to stabilize the
    divice for long term reliability.
     
  3. DJ Delorie

    DJ Delorie Guest

    FYI: please learn to cross post properly. Don't post copies of the
    same message in multiple groups, post one message addressed to
    multiple groups, like this one.

    Reasonable for what? I consider 20/10 reasonable for the fabs I deal
    with (pcb-pool can do 12/6, 4pcb can do 15/6). In your case, 20 mil
    hole with 10 mil annulus gives 10 mil clearance between copper. If I
    were to etch the board at home (or at the fabs above), I'd do 20 mil
    hole, 12 mil annulus, and 6 mil space between copper.

    Note that to meet the max dimensions, you'd need a 22 mil hole after
    plating. That leaves 11 mil annulus and 6 mil gap, or 10 mil annulus
    and 8 mil gap.

    If you want more mechanical support, extend the copper pads on the far
    side of the board perpendicular to the part's axis. They don't have
    to be round:

    http://www.delorie.com/tmp/hmc1052.html

    Another option is to stagger the holes, and bend the pins into a
    stagger pattern, with 25 mil hole and 15 mil annulus:

    http://www.delorie.com/tmp/hmc1052-2.html
     
  4. David Tweed

    David Tweed Guest

    That last one looks pretty much what Honeywell themselves do on the
    HMR3300 module, which uses the HMC1021Z sensor in the same package.
    I have a couple of these, and there really isn't much clearance
    between the round pads.

    -- Dave Tweed
     
  5. Hal Murray

    Hal Murray Guest

    Why just the far side? Why not the near side too?
     
  6. DJ Delorie

    DJ Delorie Guest

    Well, I've never had problems with parts being pushed through the
    board. Plus, in PCB, such extensions are done independently, so to
    add it to both sides would require doing the extension twice. It's
    not a big deal, I just wouldn't bother.

    Also, the larger pads increase the risk of shorts. I'd rather keep
    the risk down on the component side, as it's not as easy to
    reach/inspect under the components as it is to do so on the other
    side.

    Actually, I usually don't solder the component side of through-hole
    pins. I just solder the other side, and let the solder wick through
    the hole. I don't think the larger pad on the component side would
    add much mechanical strength in that case; all it would do (if you
    needed it) is reduce the risk of electrical disconnects due to
    off-center drills.
     
  7. DJ,
    While your comments sound realistic you are forgetting to deal with the
    diagonal sizing of the square leads. At maximum tolerances the equivalent
    round lead is 21.3mils in diameter (sq root of [19mils sq + 9.8mils sq]).
    Then you must allow tolerance on your hole both for fit and for plating
    tolerance, I would not specify these holes at less than 28mils finished hole
    size and preferrably 32mils. Then a minimum annular ring for a soldered
    through hole pad should be at least 10mils, at that it is more difficult to
    hand solder with such a small annular ring for soldering contact. So now
    your pads are at 38 - 42 mils in diameter, your space pad - pad is now 8 -
    12 mils. Now throw in soldermask expansion of at least 2 mils and
    preferrably 4 mils annular ring. You have only got 8 - 0 mils left between
    pads for soldermask web. All in all it is not a simple footprint when
    considering all design factors.

    Your other comments on hole sizing and annular rings seem to confuse
    minimum annular rings for vias, verses minimum annular rings for component
    pads. Suggesting that anyone should/could use a 6 mils annular ring on a
    component lead is not designing with good practice/reliability in mind.
     
  8. Leon

    Leon Guest


    There are SIL connectors that have a similar pitch, I've made a PCB at
    home that uses one of them and didn't have any any problems.

    Leon
     
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

-