Question about extending landing pattern traces - Page 1
Forum section: electronics / projects

author: Xpendable
author_rank: Contributor
timestamp: October 29, 2014, 06:33:10 pm
content: I have a PCB that I sell on occasion that is a shield for the standard Arduino footprint. I use some surface mount stuff on this board (along with some thru hole) and I assemble each board by hand when I get an order. I don't do a lot of these... maybe 50 a year. The one part that is an absolute pain to do is a SSOP28 (MCP23017). I can never get the right amount of solder paste on the pads... I always end up with too much. I've tried using toothpicks to drag a thin bead across the pads on each side and I've also tried a SSOP28 steel stencil. The stencil footprint is longer than the footprint on the board so this results in too much solder also. I always have to wick away or drag away some solder to fix the bridges. On average it takes me about 15 minutes just to do just this one chip.I'm getting ready to redesign my board and I'm designing the new board with an ATMega32u4 on it as well as the MCP23017. I'm still not at the point where I can afford to have these assembled for me - I still plan to do it by hand. My question is this: Would my job be easier if I extended the length of the pads for these chips so that extra paste is not as big of a deal? Like, what if I made my pads twice as long? Would that help me?

author: Precipice
author_rank: Frequent Contributor
timestamp: October 29, 2014, 06:54:44 pm
content: Is there any reason why you don't get a plastic stencil made, to do the whole board?It sounds like you're torturing yourself here, to save quite a small amount of money.If you set your location flag, people may be able to point you at a cheap supplier.(In the UK, SMTStencils will do nicely, or you might be able to find someone with a laser cutter for less?)Making the pads longer may help - if a standard stencil is much bigger than your existing pads, then it sounds like you've made them pretty small. My hand-soldering pads tend to extend 1mm further than the pin. If you have no exposed pad, that would account for a lot of your problems. But I'd still recommend a stencil, it's just so much easier than messing about with toothpicks!(Cotton buds are quite good at removing excess paste, if you need to)

author: tggzzz
author_rank: Super Contributor
timestamp: October 29, 2014, 07:07:33 pm
content: Quote from: Xpendable on October 29, 2014, 06:33:10 pmRegard this as a naive question: if the pads are extended, won't the holes in the stencils be extended, thus depositing even more paste onto the board. Obviously if the holes in the stencilsaren'textended, the question becomes void.

author: nctnico
author_rank: Super Contributor
timestamp: October 29, 2014, 07:21:31 pm
content: A good PCB package has different layers for copper, solder mask and paste (stencil) mask.I usually let PCB pads on QFP and QFN extend a little bit more so they are easier to solder by hand using a hollow tip or just a big wide tip. If cleaning up takes 15 minutes than I suspect the soldering iron is set to the wrong temperature (the right temperature is 330deg c) and/or too little flux is being used and/or the soldering tip is way too small.

author: Precipice
author_rank: Frequent Contributor
timestamp: October 29, 2014, 08:37:28 pm
content: Quote from: tggzzz on October 29, 2014, 07:07:33 pmTuning the size of the solder paste apertures is a fine art. If a board is going off to be assembled by a competent shop, I'll leave the solder paste stencil exactly at pad sizes, and it's for them to tweak the holes (I'll tell them this, to avoid the possibility of a completely insane stencil being made!). They'll do things like shift them a bit depending on which way the squeegee is running over that panel, break up large areas into smaller sections, depending on their squeegee pressure and paste type. They'll cut the stencil trapezoidally sometimes, and turn pads into bowties if they like, and for difficult stuff (wide variations in paste requirements, for instance paste-in-hole and small SMT devices on the same board), they can run stepped stencils and / or do multiple stencil runs with different stencils. It's all incredibly process specific. And then there's the insanity that is package-on-package...In short: If you're pushing the technology and want the best possible yields, this stuff is hard. If you're knocking out a few boards by hand, and can afford to inspect and fix up any problems, it's much simpler, just make the stencil pretty much pad sized. Big pads will let the squeegee bend down and scoop out some paste, so you don't get massive overpasting. Just try really, really hard to get the stencil registration right, or you'll be fighting it from then on.I've been playing with my solder paste printer this week - got an intern in writing Python to convert pick&place files into usable plot files. So far, so good, but I'm not sure I'll be able to get individual spots onto 0.4mm QFN pads, they're evil (they're pushing the limits of what I can stencil, too).Aaaand relax. This week just happens to be a 'wrestle with solderpaste' week...

author: tggzzz
author_rank: Super Contributor
timestamp: October 29, 2014, 08:58:59 pm
content: Thanks Precipice. That all seems sane, significantly extends my knowledge, and explains a few things I've seen in my limited experience.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: October 29, 2014, 11:37:26 pm
content: If you're asking how long the pads can be extended, IPC medium density rule for gull wing leads (SO, SOP, etc..) is 0.35mm past the maximum dimension, whatever that is. And you can go even more if you like -- hand soldering is a lot easier with big long pads to suck solder off of.Do edit footprints as much as you like. There is rarely, if ever, anything concrete about library footprints... in fact, in my experience they almost always suck in some way or another: bad pads, bad outline, the outline isn't the style I prefer (e.g. DIN resistor blocks instead of ANSI squiggles -- come on guys!), lack of 3D data (or the 3D data is all wrong anyway!), etc. Same goes for manufacturer recommended footprints too, argh!Have fun, and don't forget the solder wick!Tim

author: Falcon69
author_rank: Super Contributor
timestamp: October 30, 2014, 02:16:45 am
content: Xpendable,Just get a stainless steel stencil made. ELecrow, as well as many others can do this for you. Save yourself alot of headache. By a 6inch wide squeegee or a paint/mud spreader to apply the solder paste. ALl you need to do is send them a gerber file.I would also suggest getting just the stainless with no frame if you are doing these yourself. My last supplier sent them with a frame, and it's been a pain trying to work with it. Much easier to tape down a small flat piece of stainless steel, then a huge framed stencil. I think ELecrow does the stencils for about 20 bucks without the frame.Don;t try and apply that paste by hand, you'll never get the correct amount on such little pads.

author: Xpendable
author_rank: Contributor
timestamp: October 30, 2014, 03:42:51 pm
content: Quote from: Falcon69 on October 30, 2014, 02:16:45 amIt's a pain for sure for the SSOP28 and anything similar, but 0603 packages are easy for me with a syringe. I have about 25 0603 packages on my current board and I can get the paste on those pads by hand in about 1 minute. I may try the Elecrow service and get a stencil made for my current board to try it out. That's the cheapest I've seen.