Connect with us

Heat sink pads under components, extension

Discussion in 'Electronic Design' started by Joerg, Apr 11, 2013.

Scroll to continue with content
  1. Joerg

    Joerg Guest

    Question to the folks here:

    I use more and more parts that have a ground pads underneath which is
    also for extracting heat. Usually I ask the layouter to provide a big
    via in the middle so I can reach in with a Weller ETS tip to unsolder
    from underneath. I also let the pattern stick out a bit past the ends of
    the chips so I can unsolder/solder from the top without always needing
    fancy heat guns.

    Occasionally I had some groanings from producrtion folks that this is
    non-standard (which is true) and that the part may slide. Never saw any
    of that in a reflow process, but what do thee all say?
  2. Joerg

    Joerg Guest

    That makes it even tougher because then the GND plane sucks all the
    soldering iron heat away. What works nicely is to heat the individual
    pins, slide a thin valve gauge blade through (remember those?), then
    hold the tips of two Wellers onto the solder sticking out the sides and
    .... voila. Of course one would technically need a 3rd hand but I usually
    flick it up gently with one tip.

    One of our Labradors would not have this 3rd hand problem. He can
    scratch himself behind an ear with one hind leg during a dog walk and
    continue walking at our regular brisk clip on the three remaining paws.

    Those have a hard time if you have more than 1/2oz copper and the pad is
    completely covered by the IC. Best way to get it off is to also put the
    board on a hot plate but that's not going to work when stuffed double-sided.
  3. Nico Coesel

    Nico Coesel Guest

    I have been using the multiple vias methode for years. A proper 80W
    iron with a big tip does excellent for double sided boards even if the
    ground plane is continuous. Otherwise I pull out my hot-air station.
    I've found a hot air station is a very useful tool and they are really
    cheap these days.
  4. rickman

    rickman Guest

    I don't recall using any chips with thermal pads with pins on only two
    sides. The ones I see this on are mostly quad no-leads, QFN chips.
    What do you do with those?

    Regardless of how large your pad is, it is important to break the solder
    paste area into segments smaller than the pad. Do you cover the entire
    pad with solder paste, solder mask? I'm not sure exactly how you do
    this without impacting manufacturing. If the pad is covered with paste
    it might well cause the chip to float away, although the pins should
    prevent that. If you don't cover the pad with solder paste it might
    suck the paste from under your chip. If you cover the excess area with
    solder mask, it might impact thermal contact with your iron, or maybe not.
  5. Joerg

    Joerg Guest

    It's chips like this: or Series/16-TFSOP Exposed Pad 12 leads.jpg

    I am letting the pad for the bottom stick out on both sides (where there
    are no pins).

    Yep. It's the only way because the paste gets screeded onto anything
    that doesn't carry solder mask. I want solder exposure on the sides so I
    can heat things up underneath the IC from the side the IC is mounted.

    That is exactly why I am posting, asking for others' experience.

    That's what I'd like to know. Can it suck the paste out? Could it float
    away? Or will it make a solid contact and not float?

    If you cover the excess area with
    The iron would seriously burn the solder mask.
  6. Joerg

    Joerg Guest

    Do you leave some area bare so solder paste is on there? That's what I
    want to do, to be able to heat it up from the small sides (after lifting
    all the other pins) until the IC floats up.

    Which IC are you referring to? My color vision isn't that great. When
    reviewing layouts with PADS Viewer I am constantly switching colors.
  7. Guest

    We use many DFNs and SOICs with pads.
  8. I did this for the prototype, and never bothered to change it for
    production since it did not seem to cause any trouble. Despite the
    theoretical danger of the via "sucking away" the solder or whatever.

    Never had any problem, in fact it is probably the most reliable way of
    sticking down a 0.5mm pitch part I know of, and I would prefer this
    package type now. Over normal QFPs, say.

    This was total production of ~2k pcs though, so YMMV for millions.
  9. Nico Coesel

    Nico Coesel Guest

    This is why you need vias in the thermal pads. They suck away excess
    solder making manufacturing painless.
  10. Guest

    Was it this one:


  11. Joerg

    Joerg Guest

    That's what I am wondering about, if this area is larger than the bottom
    part but only at two side, and stick out the same lenth, will it still

    Is the solder mask free area on the power pad of U9 larger than
    recommended in the datasheet footprint?

    I've got too much stuff on my plate which is the main reason why I don't
    do layouts or software. Sometimes that comes back and bites me.

    Right now it's extended and exposed at two sides, making the power pad
    about 60-70% longer in chip length direction, but same extra length on
    both sides so the chip still sits symmetrical. It could not really be
    split into strips or feathers at each end because the parts are so small
    to begin with. MSOP and such.

    Worst case if an assembly house is unhappy with that they could tuck in
    the solder mask by a layer edit in the Gerbers. Not an ideal procedure
    but could be done.
  12. Joerg

    Joerg Guest

    The big via is something I've done many times before, that has never
    caused any trouble. I am just wondering about the extra (solder-pasted)
    length of the pad. It's 60-70% longer than the recommended one in the

    This unit won't be produced in more than a few thousand per year.
  13. Oh sorry I must not have read your OP properly. How about a line of mask
    to form a "solder barrier"?
  14. Joerg

    Joerg Guest

    That's a good idea but my layouter will probably have a fit if I request
    that :)

    I guess I'll let the assembly house deal with that. We use turn-key so
    if they don't like it (I will point it out to them) they can do a Gerber
    edit and we could correct the orginal data set accordingly if needed.
  15. josephkk

    josephkk Guest

    Thinking about this while reading the thread lead to the question of where
    are the forces coming from. IIRC they are viscous forces so that if the
    oversize pad extends on both ends the same amount no net force should be
    created. Then the forces on the device contacts (leads) should keep it

  16. Joerg

    Joerg Guest

    That's also my thinking. However, there are always drafts and whatnot
    even in reflow ovens so I decided to play it safe. We'll cover it but
    probably just with silk screen. Then we can scrape that off in a pinch
    and apply solder.
  17. Guest

    silk screen would work, but I've tried one pcb maker that removed
    overlapping pads so be sure to tell them it is intentional

  18. Joerg

    Joerg Guest

    Good point. I usually tell them not to alter anything in the Gerbers
    without prior approval from me. Because once a manufacturer did that,
    they "improved" a design. They had to eat the whole botched run and do a
    rush run at no extra charge.
  19. rickman

    rickman Guest

    The pins should help it center, but the large pad under the chip will do
    pretty much nothing.

    Give it a little thought. The centering works by surface tension. A
    pin is typically not much different in size to the footprint. If
    movement significantly changes the shape of the solder at the edges, it
    will create a force from the imbalance of the two sides. But if you
    extend the footprint pad far beyond the pin (or in this case the large
    pad under the chip) the change in shape will be very small for a small
    movement and there will be very little force generated.

    What John is saying makes sense. Use your large footprint pad, but add
    solder mask to define the pad area under the chip, then leave openings
    in the solder mask *outside* of the chip to lay your soldering irons.
    This will give you the proper pad area under the chip which will make
    the assembly house happy and give you areas to heat the thermal pad with
    soldering irons.
  20. All fine in theory, but I have seen "self centering" fail plenty of
    times for no reason that is obvious to me.

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