QFP solder bridging problems - Page 1
Forum section: electronics / general

author: ubbut
author_rank: Regular Contributor
timestamp: February 08, 2020, 09:31:46 am
content: Hi,I have been doing prototype boards and small production runs for the last years and usually have very good results, but still struggle with 0.5mm QFP.I use Loctite GC10 paste and reflow oven. Stencil are are stainless steel, both framed and non-framed. I have issues when placing parts by hand and also when using the PnP.Way too many QFP need rework, I rarely encounter a single IC without a solder bridge.For the boards I use 4mil solder mask expansion. In theory this should leave a 0.3mm solder mask strip between the pins. Hover looking at the bridging under the microscope shows the bridges are not necessarily at the end of the pins (where they touch the board) but often 'higher up' and closer to the IC. Too much paste?I don't have the same problems with 0.5mm QFN..Any suggestions to what I might try to optimize my process?thanks

author: thinkfat
author_rank: Unknown
timestamp: February 08, 2020, 10:06:33 am
content: Totally agree with blueskull. I ended up redesigning a board because I was sick of soldering 0.5mm QFP. QFN with center pad rules and is even more compact, takes up less board area.

author: ubbut
author_rank: Regular Contributor
timestamp: February 08, 2020, 10:35:39 am
content: Quote from: blueskull on February 08, 2020, 09:47:53 amGood suggestion! I assume you wouldnotalso extend the paste opening?I agree with using QFN for future projects.I now however have the situation with an existing board (Part does not exist in QFN anyways).Wonder if there is anything I can do to improve the existing process - after all, assembly houses have to deal with QFP on a daily basis and somehow manage?

author: SMTech
author_rank: Frequent Contributor
timestamp: February 08, 2020, 02:54:37 pm
content: I don't think you need $100k equipment, not least because you can get 3 new fully automatic printers for that kind of money.I print lots of board using a manual printer that use 0.5mm QFP & TSSOP sometimes you do get bridging it tends to be on specific boards where whoever designed it has followed slightly different rules for the stencil apertures.The cause is pretty much all in the printing, you really need the stencil to be in a frame with good tension that sits nice and flat against the PCB* and 100/120 micron is about the right thickness. You can apply a reduction to the aperture size, although there is a limit to what you can do at 0.4/0.5mm pitch.Make sure the paste is decent, in-date, properly stored and well mixed, clean the underside of the stencil every 5 prints with a treated stencil wipe and make sure the paste is printing with a rolling action instead of being pushed through the holes by an acute angle and excess pressure. You can also play with the footprint in general as long as there is enough pad& paste under the device to at least create a "heel" fillet you can experiment with what works for your method.*This is why I don't use the framed stencils from JLC/PCBWay, they are not totally flat, the tape and bonding material gets too close to the PCB meaning it can space the stencil away, the surface is poorly finished (even the "polished" ones) and the apertures seem more likely to release paste poorly. For small one-off batches that's fine and still better than no-frame but otherwise I consider the £100-£150 on a proper stencil, money well spent. They also don't seem to pay any attention to requests if you put them in the stencil section.

author: jmelson
author_rank: Super Contributor
timestamp: February 08, 2020, 06:30:34 pm
content: Quote from: ubbut on February 08, 2020, 09:31:46 amYou need to reduce the stencil aperture for smaller pitch parts. I go down to about 70 % linear dimension for 0.5mm pitch, so that isabout a 50% area aperture. (It is kind of rough, as I am also correcting for over-etching in my stencil manufacturing process.)I also use .003" brass shim stock to make my stencils, that is about .075 mm. Too much solder will guarantee bridging. Also, the componentalignment is fairly critical. If the parts are misaligned, the chance of bridging increases. I do lots of boards with 0.5mm FPGAs and GC10,and with the above adjustments, I rarely have the bridging issue. But, I DO ADMIT, it took a while, and a number of revisions on my stencilaperture rules, to get it right!Oh, one other issue is alignment of the stencil with the board. For SOIC parts, bare-eye visual alignment is fine. For 0.5 mm QFPs, you need to use a microscope or at least good magnifier to make sure the QFP apertures line up with the IC pads. Misaligned solder paste will definitely cause bridging issues!Jon

author: SMTech
author_rank: Frequent Contributor
timestamp: February 08, 2020, 06:58:29 pm
content: Quote from: jmelson on February 08, 2020, 06:30:34 pmHow much misalignment matters depends a bit on just how misaligned you are, 25% of the pad off and you're probably fine as long as there isn't too much paste, if you are placing manually in which case the best thing to do is align your component with the paste not the pad and let the solder do the rest. Any more than that and with 0.5mm you run the risk of the device soldering itself exactly between pads.I don't find 0.5mm that hard to align by eye (I might if my aperture reduction was as aggressive as jmelsons) except in the instance of a white PCB with ENIG finish, which becomes very hard to see. 0.4mm however certainly strains the old eyeballs . You also need to be very sure of your PCB fixture, if anything can bend or shift, it will affect it.I've written this elsewhere but if you radically reduce the stencil thickness to solve your bridging issue there's a chance that some QFPs with a center pad will not make contact with the paste deposited from an overly-thin stencil.Your end result should have clearly visible solder fillets on all joints with some solder flowing up the side of the part and forming a nice ~45degree angle. If they merely "look soldered" there isn't enough paste.

author: ANTALIFE
author_rank: Frequent Contributor
timestamp: February 12, 2020, 03:09:28 am
content: Show us ya PCB footprint

author: ubbut
author_rank: Regular Contributor
timestamp: February 20, 2020, 09:35:43 pm
content: Followup:After reading the suggestions presented here I tried very hard to get the paste applied as precisely as possible and now have in fact much better results

author: liteyear
author_rank: Regular Contributor
timestamp: May 06, 2023, 11:54:45 pm
content: Quote from: blueskull on February 08, 2020, 09:47:53 amI guess blueskull is not with us any more, but I wanted to follow up on this point. I often find default paste orifices result in far too much paste, but there's lots of contributing factors. The one mentioned here though I think is an important one:QuoteThemanufacturer recommended land patternfor a 32 pin TQFP centres the pad around the contact area of the pin. The footprint in the KiCad library follows this exactly, which leaves around 0.5mm of the pad extended towards the interior side beyond the pin itself.I tried reflowing an ATmega328P and an ATmega16U2 (no prizes for guessing what my design is based on) with this footprint and suffered this phenomena:Even after clearing off all the visible bridges with wick, I still had a short. Pulling the chip revealed a build up of solder ridgesunderthe pins, which you can see in the photo on the top left 3 or 4 pads.So I'm tempted to shorten each of these pads next time 'round. Is there a possibility this will cause other problems, say because the chip will be unevenly pulled during reflow?I will also try a slightly thinner stencil (this was 0.15mm), and probably a global 10% reduction in paste orifices. But it's hard to predict the overall impact.More photos availablehere.

author: dkonigs
author_rank: Regular Contributor
timestamp: May 09, 2023, 02:33:39 am
content: Quote from: liteyear on May 06, 2023, 11:54:45 pmI recently did a run with an ST component in an almost identical package (they call it LQFP-32, but the dimensions match up), and thedatasheetfrom ST gives a recommended land pattern with shorter pads. I've never had any bridging problems on this part.On a different project, I used a different ST part that came in an LQFP-64 package and originally went with KiCad's default footprint. I had no end to bridging problems, so I'm planning to switch to ST's shorter-pad land pattern for the next prototype of that project.

author: liteyear
author_rank: Regular Contributor
timestamp: May 30, 2023, 04:50:59 am
content: Thanks for the pointer on the ST land pattern. See attached a comparison: original for pins 1, 4 and 5. ST recommendation for pin 2. And what I think I'll run the gauntlet with for pin 3. It's a further 0.1mm shorter, and offset to maintain the same outer edge as ST.

author: dkonigs
author_rank: Regular Contributor
timestamp: June 16, 2023, 01:34:41 am
content: Yeah, paste can also play a big role.Footprint tweaks aside, the vast majority of my post-reflow solder bridging problems pretty much vanished the moment I switched to using Loctite GC10 solder paste.(Before that I was using various pastes ChipQuik sold in syringes, some of which needed refrigeration. It always tended to get a bit oozy before reflow, whereas the GC10 seems to pretty much hold its shape as I'm placing parts.)

author: liteyear
author_rank: Regular Contributor
timestamp: August 09, 2023, 03:09:13 am
content: Much better results with the shorter pads. Not only was the frequency of bridging far lower, but when there was a bridge I could fix it every time without removing the part.But even with a 99% success rate per pin, when you have two 32 pin QFP's on the board, that's still lots of boards that require rework.Quote from: karpouzi9 on June 15, 2023, 06:26:29 pmThis is a persistent doubt, and I'm always pedantic about paste. I always buy paste for the job (never store it) and move carefully from recommended paste to recommended paste. Technique and preparation has a lot to do with it too, so results vary, and I've spent years tweaking the eighty or so variables and looping around the long feedback loop.I have an upcoming post analysing paste, once I collect some quality data. There's a previewhereand a bit of discussionhere.In the meantime, I have another board about to go out that has the two TQFP-32's from before, and adds a LQFP-32! So I'm motivated to get it right. After looking at the LQFP footprint (which despite having exactly the same x and y dimensions, differs a little), I incorporated two more minor tweaks:Reduce pad width from 0.55mm to 0.5mm. Not much difference in pad area, but visually seems to increase the spacing between pads by a bit.Add 0.1mm radius corners. Manufacturer recommendation is 0.05mm, KiCad footprint uses 0.125mm. I figure 0.1mm will remove a little of the useless corner area, reducing the quantity of paste and lowering the reflow stress in the corners, and also make release from the stencil a little more consistent (I saw evidence of wall sticking on the first application after a clean).See attached the same pad comparison image as before, except pad 4 is the new pad. I've also included one annotated with the nominal (all dimensions are about ±0.15mm) pin foot size, but keep in mind the pin bends away from the board on the inside edge.Another experimental variable is having a stencil (paste mask) different to the solder mask. Not recommended in the OEM footprint, but seems like a logic thing to do. Only, I'm not prepared to open that box yet because my PCB fab (JLCPCB) ignore the paste layer by default and do their own adjustments off the solder mask. Seeherefor that complexity nest I'm not yet willing to poke.

author: DavidAlfa
author_rank: Super Contributor
timestamp: August 09, 2023, 04:08:23 am
content: Judging the last picture, it seems there's a bit too much solder in these resistors/caps, I'd say 25%.Not an issue there, but definitely will be for small parts.Or have you touched with manual soldering?

author: liteyear
author_rank: Regular Contributor
timestamp: August 09, 2023, 06:37:14 am
content: Quote from: DavidAlfa on August 09, 2023, 04:08:23 amHeh, it did cross my mind. But they're bog standard footprints straight out of the reflow oven. Though with a 150 micron stencil and withsolder beading treatment. Haven't had an issue with them but good to know thankyou!Meanwhile, as I prepare this board to go out, I have similar bridging doubts with the standard 0.65mm pitch SSOP footprint too. Again, this is based on OEM recommendation, but I'm not going to suffer through another board spin this time. Second attachment shows pin 1 with my QFP-inspired pruning. Why wouldn't I?

author: Psi
author_rank: Super Contributor
timestamp: August 09, 2023, 08:22:41 am
content: What thickness stencil are you using.I found when I went to 0.08mm it helped a lot. The PCBway default is 1.2mm and IMHO its way too thick.Combine that with reducing the aperture openings on the solder paste layer and that fixed my issues.Oh, and it helps to get a very clean paste transfer onto the PCB, not smudged.And placing the part on the pads correctly not off-center and then moving it with tweezers which also smudges the paste. However these last 2 things matter MUCH less than the first things above (0.08mm and reduced paste aperture)

author: liteyear
author_rank: Regular Contributor
timestamp: August 09, 2023, 11:03:27 am
content: Quote from: Psi on August 09, 2023, 08:22:41 am0.15mm. I thought it was too thick, but it's well within the widely published recommendations for the aperture sizes I'm working with.Example. I wonder if you're right and those recommendations are whack? I feel like a cross-the-board reduction in paste wouldn't be a bad thing... so why the standard recommendation based on aperture size? Doesn't make sense for a board with mixed aperture sizes.Quote from: Psi on August 09, 2023, 08:22:41 amYeah good point. It's tricky sometimes. Fortunately I haven't found this to have a significant impact, within reason. At one point, if I smeared some paste realigning a part I would clean it off and start again. As I build up my good-result database, I've started to allow one or two adjustments and some bad smear on the less fussy pads. Particularly because the automatic pick and place mooshes the paste placing the part down anyway, and that doesn't seem to cause major issues.PS. I mentioned the stencil thickness in my previous post, but it also gobbled my URL. I fixed it up: trial and error revealed that I needed to add a redundant "www." after the "https://" !

author: Psi
author_rank: Super Contributor
timestamp: August 09, 2023, 11:43:36 am
content: Yeah, i've heard others say 0.15mm as well, but it just puts way too much paste on the board for me.Then I get bridges.It might be something to do with my technique using the Squeegee, maybe I compress the paste more than I should. But I find I need that downforce to keep the stencil flat on the PCB.(I think the proper paste machines have more of a horizontal sliding action with very little down force)I use 0.08mm or sometimes 0.1mm thickness stencils and T4 or T5 paste (T number is the ball size)I also try to stay away from chipquik brand paste.Had to many bad tubs of it. It seems too inconsistent. Sometimes you get a good batch and other times it shit.I usually get Kester, but you pay twice as much.I also tend to find I get a better paste transfer when the solder paste is colder.After it gets warm it gets a bit too runny and doesn't holds its shape as well, which makes the stencil to PCB transfer quality get worse.

author: DavidAlfa
author_rank: Super Contributor
timestamp: August 09, 2023, 03:15:10 pm
content: Notice how your smd passives would sit at 150-175%