Stencil Apertures - Page 1
Forum section: electronics / general

author: jpanhalt
author_rank: Super Contributor
timestamp: March 29, 2020, 05:47:25 pm
content: My current design is not particularly small. IC's are TQFP, MSOP, SOT23-5, and 805's for other things. This will be the first time I have ordered or even used a stencil.I use Eagle 7.2. Several sources (some board houses and Adafruit) recommend shrinking the "cream" (solder paste layer) if it is used for the stencil to prevent bridging and other problems. The default cream layer that Eagle uses is the same size as the pads.Is it necessary to shrink the cream layer? Adafruit uses ViewMate to shrink aperatures, but that is expensive. I could not find a ULP to do it.Will using a thinner stencil, say 0.010", be better than a 0.012"?Edit: I guess I am really a noobie at this. One vendor offers SS stencils in 0.003" to 0.008" thickness. It seems those thinner stencils would solve any excess solder paste concerns. Comments?

author: ANTALIFE
author_rank: Frequent Contributor
timestamp: March 30, 2020, 12:35:32 am
content: I'm quite new to stencils as well, but from my understanding for your complexity you want:10% aperture reduction3mil thicknessStainless steelAlso here are a couple of good resources:https://smtnet.com/library/files/upload/Stencil-Design-for-Lead-Free-SMT.pdfhttp://triembed.org/blog/notes-about-osh-stencils/

author: SMTech
author_rank: Frequent Contributor
timestamp: March 30, 2020, 11:03:10 am
content: .003?! Nah, maybe 120/125micron (.005) or if your QFP are 0.5mm pitch you might drop down to .004. Even aperture reduction can be somewhat optional, it depends a bit on your land patterns (seem to be multiple in-house & formal standards in use) and , however 10% is typically pretty safe, giving you a reduction without risking it being excessive. you should be able to define your paste layer ratios in your component def. However you should also be able to tell your stencil fab "please apply 10% reduction" and they will do it for you.There are formulas out there that you can use for stencil calculations but manual printing adds a little flavor that spoils those.

author: jpanhalt
author_rank: Super Contributor
timestamp: March 30, 2020, 12:07:59 pm
content: Thank you both for the advice.@AntalifeThose are nice resources. I had pretty much decided to get the stencil made at OSHStencil regardless of where the board is made. It offers more choices than the lowest-cost board houses in China offer. It is also located in the US (as am I) so a lot is saved on shipping. As many have noted, the shipping cost for stencils from China can easily double the total cost.@SMTechYou sound like you have experience, or maybe it is just your user name.General:I am not new to soldering (>60 years) and have been doing mostly SMD since the late 90's. Everything has been by hand. That is, this is my first venture into reflow, and I intentionally designed the "draft" board so that if reflow is a complete failure for me, I can do it by hand. Hence, the 805 and leaded packages.Some manufacturers just give a pad outline with no guidance for reflow soldering. TI offers both. Here is a link to TI's advice for small leaded packages (TQFP and TSSOP):http://www.ti.com/lit/an/slma002h/slma002h.pdfFor leaded packages with some standoff, TI references JEDEC (about page 10):QuoteThis table caught my eye:The pad size is 5.19 x 5.19. Thus, a 1:1 aperture with a 5-mil stencil is recommended and a thinner stencil results in an aperture that is actually larger. That is consistent with the above quote. However, if you start reading on page 1, for a 0.65 pitch leaded package, TI recommends a 17% reduction in aperature width ( 0.25 mm for a 0.3 mm pad) and a 3% reduction in length.Tentative conclusion:I will get a 5 mill stencil and use 1:1 aperture.That should suit my leaded packages. If it is too much for the 805 passives, a little solder wick will help. BTW, I use leaded solder and that may also affect choice of stencil aperture. I am not sure OSHStencil offers a shrink option in the price. If so, please let me know whether you would still recommend doing that. If offered, I suspect it is either all or nothing. That is, it cannot shrink just the apertures for the 805's and leave everything else full size.Since I almost always use my own component library versus something downloaded or in the Eagle library, changing the cream layer would not be all that hard to do. It is just another variant and a few clicks on the board.John

author: jmelson
author_rank: Super Contributor
timestamp: March 30, 2020, 07:10:57 pm
content: I have done over 2000 boards in my homebrew setup. I make my own stencils out of .003" brass shim stock, with photoresist and FeCl etching technology. I use a pretty heavy aperture shrink on the smaller pitch devices. This is partly to compensate for over-etching of the apertures,but also to reduce solder paste to prevent bridges. The 0805 and up passives are no issue, although you can get some solder balls next to the parts.SOIC ICs are no problem either. But, anything smaller and you have to worry about the apertures. 0.65 mm requires a little reduction,0.5 mm requires even more reduction, maybe cutting area to half the pad's area. Also, reducing the pad width to about the same as the lead width can help.Jon

author: jpanhalt
author_rank: Super Contributor
timestamp: March 30, 2020, 07:19:09 pm
content: May I ask how you do the reflow? Oven, hot plate, hot air or a combination of the last two?

author: jmelson
author_rank: Super Contributor
timestamp: March 31, 2020, 06:52:43 pm
content: Quote from: jpanhalt on March 30, 2020, 07:19:09 pmI have a Philips CSM84 pick and place machine. I do manual stencil printing. After placement, Iput the boards in a big GE toaster oven with a thermocouple ramp-and-soak controller.I poke a tiny thermocouple into a plated through hole on one of the boards, and startthe temperature ramp. I do a ramp to 180 C, hold for one minute, then ramp to235 C, hold for one minute, and cool down. I've forgotten the ramp rate I use,but it is a couple minutes to 180 and then a couple minutes to 235.Solder paste is GC10, which has proved to be AMAZINGLY good! I tried a number of others, somewere mediocre, some were totally HORRIBLE.Jon

author: montemcguire
author_rank: Regular Contributor
timestamp: March 31, 2020, 06:58:57 pm
content: Quote from: jmelson on March 30, 2020, 07:10:57 pmIn my experience, solder balls next to the components (graping) is the result of an insufficient reflow profile, specifically too short of a thermal soak time. Make sure that the reflow profile you use matches what the paste vendor says should be used. I use an IR preheater with a hand hot air wand to reflow, and while you can get everything to flow sufficiently without the full duration of preheat and soak, graping is the usual result. I was so paranoid about burning off all of the flux or cooking the components that I tended to short-cut the higher temperature soak time, using hot air too soon in order to get the board to flow quickly. One time, I actually followed the programmed profile in the IR machine and didn't use air until I was well past the preheat and soak cycles and it worked much better. It made sense when I realized that only just now was I following the recommended profile.I saw in your post that you use a 180C soak, which might be too low. I'm using a 90 sec 200C soak with lead paste, so that's proportionally a lot higher, and with the full soak, I get no graping.QuoteI use commercial laser cut stencils and find that there is no need to use anything but a 1:1 pad for small pitch, including 0.5mm. I've examined the stencils with a microscope, and while the apertures do have some error, it is generally small, and certainly not the result of any undercutting. I'm using a lot of PCBway boards these days, and measuring those small pads, I find that they are sometimes made smaller through over-etching, but not by a huge degree. Maybe this too is what motivates reducing the aperture size - examining the stencil and PCB for under/overcutting is probably in order.I use PCB Library Expert to design the footprints, since it's simpler than trying to parse out all of the IPC recommendations, so the pad geometry is generated there, and then used with a 1:1 paste geometry, except for larger pads such as die attach pads and thermal tabs. PCBLE will make a nice checkerboard pattern to get the right paste percentage, which is generally around 70-75% of the pad area. I use 5 mil stencils, so large DAPs need to have a paste reduction to get the component to "float" to the right height to make proper fillets for the other small pads on a package. There's a TI SO-8 with a DAP in the center, and that required some complex calculations to determine the amount of solder needed to barely float the package body while creating proper fillets for the gullwing pads.A thinner stencil would certainly make the 0.5mm parts easier to manage, but the larger DAPs would need greater than 100% paste area, which is not generally possible. So, 5 mil it is, with quality paste and the proper profile, and it seems to work.

author: SMTech
author_rank: Frequent Contributor
timestamp: March 31, 2020, 09:11:44 pm
content: You can cause flux to boil and hence spit out solder balls but its far more likely to be caused by paste trapped under the device, too much paste with nowhere to go, poor or outdated pad/footprint design can contribute. An easy fix is to homeplate the apertures if you see it on passives, excess paste can also come from poor stencil tension (e.g no frame or crap frame) or poor gasketting between the PCB and the stencil squeezing paste between the two during print.No idea what paste you are using but our lead-free paste has a 60-90 second soak between & 150&180C, leaded would be more like 140-160 given that would peak at 205 for reflow.I have seen chips like QFPs with a centre pad fail to make contact with the board if you use too thin a stencil.

author: jpanhalt
author_rank: Super Contributor
timestamp: March 31, 2020, 09:20:57 pm
content: Thanks to all. After the initial comments, my quandary was whether to get a 4 mil or 5 mil stencil at 1:1. With a little more research on OSHStencils, it will probably be 4 mil SS at 1:1. If that fails, at least the part will stick and I can go back to my tried and true method of hand soldering with solder wick.