PCB Pad Design for QFN and MLP(Q) Packages

Discussion in 'General Electronics Chat' started by jpanhalt, Oct 2, 2016.

  1. jpanhalt

    Thread Starter AAC Fanatic!

    Jan 18, 2008
    5,683
    900
    I am now at the point with my lightning detector(s) to design my own board. The requisite chip (AS3935) is an MLPQ, which is very similar to the QFN with a central heatsink and ground plane connection.

    Recommended layout (http://cds.linear.com/docs/en/packaging/Carsem MLP users guide.pdf ) is to use "non solder mask defined" pads (NSMD pads). That is, don't put solder mask between the pads. The alternative is "solder mask defined pads" (SMD pades) which has each pad separated by a microscopic line of solder mask. I understand the argument for using NSMD pads when doing reflow soldering.

    My plan is to hand solder the chips, which are 16-pin, 4 mm x 4 mm with 0.65 mm pad spacing. Does anyone with experience have a recommendation for which type of solder mask to use? I have experience using larger leadless packages and simply heated the pad and exposed lead on the side of the package while wicking the solder under the device. It seems to me that with hand soldering the solder mask define pad might be preferable as it should help avoid bridging under the chip.

    My solder is 63/37 tin lead 0.015 with rosin core.

    John
     
  2. ErnieM

    AAC Fanatic!

    Apr 24, 2011
    7,386
    1,605
    63/37 w/rosin core? Stranded solder? Ummm...

    I have hand soldered a few QFN chips, though with fewer leads and I don't remember if they had a central pad. I did not use an iron but a hot air pistol and solder paste consisting of tiny balls of solder in a flux suspension.

    Such a set up would (or may) work for the center pad too, you just preheat the pad and the chip bottom together then plod the chip in place, then run hot air around the edges. Once all the solder is liquid surface tension pulls the part into precise placement.

    If I was going to use a conventional solder tip iron I would extend the pads well outside the chip area so my tip could touch it. Then solder could be semi-forced to flow under and touch the device pad. I would completely forget about getting the central pad to reflow, you just have no access to it.

    Solder mask is not going to help or hurt this process.
     
  3. SLK001

    Well-Known Member

    Nov 29, 2011
    813
    225
    I've put parts like this down with a heat gun. I first applied solder to all the pads, then applied flux to both part and pad. When applying the solder, you need to be careful to apply it equally on all the pads (I sighted across all the pads looking from the side). Also, do not apply too much solder to the center pad or it will prevent other pads from making contact - too little solder is also bad, because it may not make contact.

    Set the part on the pad and with your heatgun held high above the board, slowly bring the board and part up to temp by starting high and slowly move the gun down. You want to approximate a reflow cycle with the heat gun. When the solder hits liquidus, you should be able to see your part pull itself into proper position - you can take a dentil pick and push the part and it should return to its proper place (it's floating on the liquid solder and the surface tension keeps it in place). Once here, move the gun back up slowly and allow the board to cool to room temp.

    If parts are already placed on the board, use kapton tape and aluminum foil to build a heat isolation area around the chip.

    Oh, and solder mask is not needed on the exterior pads, but it can be used.
     
  4. jpanhalt

    Thread Starter AAC Fanatic!

    Jan 18, 2008
    5,683
    900
    I am primarily interested in hand soldering with a conventional, fine tipped (conical) iron. Won't rule out using hot air. I have a hot-air plastic welder that is not temperature regulated, which would probably work, but in reality I would probably just bite the bullet and buy a station -- seems like an awful expense for soldering just 32 leads.

    Schmartboard (schmartboard.com) makes breakout boards for small parts. Their boards have grooves for the leads to help center the chip. I have its QFN board, but the pads extend too far beneath the chip and might contact the exposed ground pad (EP pad) there. There is a large plated through via there that measures about 31 mil finished diameter (a # 68 drill barely passes). In theory, one could solder through that hole. There is no copper pad in the middle on the chip side of the board

    I have a couple of drafts for the Eagle package with various versions of the pad shape, vias, and names for the EP pad. This version has the center EP set as a numbered pad. That should help in the final layout error checks. I have extended the pads 1 mm beyond the outline of the chip (grid = 1 mm) to allow hand soldering and filleting. That seems a bit large, but is smaller than what Schmartboard uses.

    My concern now is soldering to the center EP without using solder paste. Some people show 4 vias there when using reflow, Smartboard uses a single large via dead center. I am leaning toward the latter. Here's one of the 3 versions I am working with. No vias are shown, and the cream layer, while shown, can be ignored if I follow my current plan. The little circles on the cream are locators/reminders to put vias there for reflow. As mentioned, the EP in this version has a proper pad number (17), which will mandate a ground connection to it in the design to avoid an ERC error. That decision is being reconsidered. Alternatives are a simple rectangle or polygon on the top layer built up with the appropriate stop and cream layers.

    upload_2016-10-4_6-25-40.png

    John
     
  5. kubeek

    AAC Fanatic!

    Sep 20, 2005
    4,670
    804
    If you are doing your own boards, it is best to make a single large via under the thermal pad, and solder it from the bottom side after you get the normal pins right.

    It can also be sodlered with normal soldering paste, preheat the board from the bottom side and use hot air gun, then after the solder starts flowing push the package into the board to squeeze out excess solder from the thermal pad, but be careful about moving the chip out of alignement in the process.
    Then using soldering iron and liquid flux touch up the pins to get good connection everywhere.
     
  6. jpanhalt

    Thread Starter AAC Fanatic!

    Jan 18, 2008
    5,683
    900
    Since I get three boards, I will be experimenting. I am definitely leaning towards the one big via. I can make small, tinned copper slugs. One thought was to put a dab of solder on the end, stuff it in the hole, then heat until it settles. My worry is that a single via without a vent (at least other vias do that function) will act like casting metal without vents in the the mold and not flow well.

    These parts tend to push the limits of board makers. Another concern I have is that with the default Eagle setting for solder mask, the mask between pins may be too narrow for the board maker. I can easily get it to almost 10 mil by decreasing the pad overlap. I read on the Element14/Eagle site that there is no rule that says the solder mask can't be smaller than the copper pad. In fact, some designs dictate that. Here is a revised version that shows both sizes of solder mask. Pads on the left have the reduced mask (about 0.05 mm larger all around),

    upload_2016-10-4_9-18-15.png

    John
     
  7. kubeek

    AAC Fanatic!

    Sep 20, 2005
    4,670
    804
    The chip you are using does not produce any significant amount of heat, so the thermal pad here is mainly used to get nice solid ground for the chip. You you don´t need to worry about having the whole area connected to the ground plane as the chip has a copper plate anyway. All you need is that one single connection to ground which the single large via will provide.

    As for the solder mask, most manufacturers will have trouble with narrow strips you leave masked and might delete them manually. Also be careful that the positioning of the mask is often quite sloppy and with fine pitch parts you could end up with mask on the pins instead of between them. Usually you see parts with no mask between the pins, just between the pins and the thermal pad.
     
  8. jpanhalt

    Thread Starter AAC Fanatic!

    Jan 18, 2008
    5,683
    900
    Not having soldermask between pins is the so-called NSMD (non-solder mask defined) arrangement. For solder paste, the stencil is made smaller than the pad. For hand soldering, it seems having some soldermask between pads is preferred. Just checked Oshpark's actual design rules for masks. Eagle default is 4 mil, Oshpark's is 3 mil around pads. The former created a problem with minimum separation. The latter gives me 7.8 mil (about 1/128";) ) of solder mask. Narrow, but it should do the job. Fortunately, the design is so symmetrical that I only need to re-define two of the SMD pads for the changed soldermask.

    Device draws 350 uA when working (1.75 mW). Heat is not a problem as you say, but I do want to be sure I have a good ground.

    Fall projects on the hobby farm are lined up for today. Will have to put off more work on it until evening.

    John
     
  9. schmitt trigger

    Active Member

    Jul 12, 2010
    36
    7
    What I've done in the past to solder the central pad without paste, is to liberally apply flux on the pad.
    Then with a very thin solder wire apply a little solder on the pad itself, and as it becomes liquid spread it evenly across the surface. The thing here is to already have solder deposited across the pad.

    Once that it is done, place the IC on the PWBA, which has more flux applied. Please note; the PWBA's pads must be tin plated. Bare copper won't work.
    Then with a hot air gun, heat the the board until it reflows. You require to push on the IC's top with a long screwdriver to apply force such that the liquid solder spreads evenly.

    Allow it to cool. Once that the IC is secure, you can start soldering by hand all the remaining pins.
     
Loading...