Are my stencil apertures too small?

[HwAoRrDk]

I have some 0.5mm pitch parts on a board - a QFN and an FFC connector - and I'm concerned that my paste stencil apertures for the pads on these parts are too small. I hate dealing with these fine-pitch parts as I've always had problems in the past. I want to put some effort into making sure I've really got things right this time.

I've been reading IPC-7525A, where it talks about the ideal aspect ratio and area ratio for stencil apertures; the reason being, as I understand it, so that paste easily separates from the stencil and stays on the board. Aspect ratio being the ratio of aperture width to stencil thickness, and area ratio being the ratio of aperture opening to aperture wall area (i.e. the vertical sides of the aperture). As a general guideline, the aspect ratio they give is >= 1.5, and area ratio >= 0.66.

The pads on the QFN are 0.85x0.26mm, and the FFC are 1.2x0.3mm. With my default paste shrink of 0.05mm, that gives apertures of 0.75x0.16 and 1.1x0.2. The ratios for those are 1.07/0.44 and 1.33/0.56, which falls short of the recommended values.

If I go ahead and use these aperture sizes, am I going to definitely have problems with paste application?

In order to meet the guideline figures, I would need to reduce my paste shrink on the QFN to zero (i.e. so aperture same size as pads) and 0.03mm for the FFC. The former worries me as it seems like too much paste for such a tiny pad. I don't want to then have bridging problems because of too much paste!

In the IPC-7525A document they also have charts of acceptable area ratio for varying stencil thickness. I plan to have my stencils made at JLCPCB, and their default stencil thickness is 0.15mm (approx. 6 mil).



My revised aperture size puts them both just about on the middle red line for "Electroformed or Laser" stencils. I presume the different stencil fabrication techniques correspond to varying levels of roughness of finish of aperture, which is the only thing I can think of that would affect paste release. I believe JLCPCB stencils are laser cut, so that chart data should correspond, right? JLCPCB also recommended a different, optional, polishing process ("Etching Polishing") for component pitches of 0.5mm or less. They explain it as having a de-burring effect. So, if I order my stencil with that option, it should definitely put me well within the red line on the graph?

[SMTech]

Laser cutting is considered to give a straight edge, with vertical walls as the laser blows tight though. Etched stencils have shaped sides, that shape depends on if it was etched from one side or both. Traditionally etched stencils are considered preferable for fine pitch, laser cut stencils should ALWAYS be polished after cutting. Modern commercial stencil may mix technologies or have more advanced laser cutters.

If you compare a PCBWay/JLC stencil with a proper commercial standard one, you would notice the paste release is noticeably worse, certainly in the case of the the PCBWay ones, the so called "polishing" is some half arsed effort that looks like someone rubbed it manually with some fine grit paper.

I would experiment with % aperture reductions rather than a fixed number, also experiment with aperture reduction shapes such as homeplate, see if some work better for you than others. QFN is really not that prone to bridging and is fairly safe @ 1:1 and you certainly want to keep your aspect ratio inside those guidelines. If your stencil thickness prohibits that, what you may actually need is a stepped stencil. By contrast TSSOP @1:1 really doesn't work, those big fat leads relative to the pitch make the package very sensitive to paste thickness, as well as environmental conditions and can become a magnet for shorts even when all your alignment looks spot on.

[HwAoRrDk]

If you compare a PCBWay/JLC stencil with a proper commercial standard one, you would notice the paste release is noticeably worse, certainly in the case of the the PCBWay ones, the so called "polishing" is some half arsed effort that looks like someone rubbed it manually with some fine grit paper.

PCBWay stencils not great? That would explain some of my previous troubles... It's mostly with PCBWay ones that I've had problems.

I would experiment with % aperture reductions rather than a fixed number, also experiment with aperture reduction shapes such as homeplate, see if some work better for you than others.

Unfortunately my PCB software doesn't cater for percentage aperture shrink, just an absolute value, but I can do that on a per-pad basis. Same with aperture shapes - limited to matching the pad shape. If I want alternative shapes (other than segmentation), then I'd have to draw them manually (which I sometimes do for ground pads). I am using rounded corners on all pads, though.

QFN is really not that prone to bridging and is fairly safe @ 1:1 and you certainly want to keep your aspect ratio inside those guidelines.

Really? That's been like 80% of the problems I've had with QFNs - bridging. Which is why I'm hesitant to go with a 1:1 aperture size for fear of putting too much paste.

[SMTech]

I see far more PCBWay ones than JLC, I hate them both. However the JLC ones I have encountered, in the larger sizes seem to be build around a more robust frame. I wouldn't like to say the surface finish or apertures are any better, although JLC stencils supplied by customers seem typically have a U shaped homeplate applied by default.

When we buy proper stencils, we can specify things like a 10% reduction and aperture shapes, hatching on large areas etc, if we believe the board may have other challenges we can ask for feedback and advice, that might result in things like a multi-level stencil. Some of them (re)generate a paste layer from scratch, or claim to.

I would be far less surprised at seeing a dry joint on a fine pitch QFN due to paste release due to poor cleaning than a short, I quite like them as a package and we find they have a good success rate while being more likely to arrive undamaged when you are buying small qtys. Get too much paste on the enter pad tho' and you can get a whole heap of problems.

[selcuk]

If you are planning to order from JLCPCB, I can recommend you to choose electropolishing. I've recently made a stencil and boards manufactured with a minimum of 0.35mm pitch QFNs and didn't have any issue. You may check the photo. The footprint is QFN48 5x5.

If you order sand polishing, you can clearly see the scratch marks on it. I haven't tried it for this component but I used it for a 0.5mm pitch QFN for hand prototypes and I didn't have any issues. But I'm not sure for mass production.

[loki42]

Is there a manufacturer you recommend for stencils?  What's a decent price for an framed non stepped stencil?  Do you use nano coating?

[SMTech]

In the UK, major suppliers of stencils are Alpha (who I assume have a global presence), ASMPT (global -own the Vectorguard system),Tecan, Tannlin (invented the Vectorguard system). At various points we have used them all over the last 20 years, except ASMPT. These days I think they all have an online portal to submit files, they all use pretty standardized pricing, have an approval process before cutting and will give advice if you need it.

Framed stencils can vary a bit between suppliers. However a typical Vectorguard (needs a tensioning frame) stencil seems to be about £165 regardless of where from and you would add about 50% per step if they were needed. Some alternatives to Vectorguard might cost less (no aluminum sub-frame) or more due to licensing cost, VG is available everywhere.

We have not tried a nano coating, I don't think we do the volume to generate the metrics to say it works or not, and neither do we do all that much with very small apertures. There are also gold coatings or Nickel stencils, I haven't tried either, although I have tried a nickel Squeegee which did seem to work quite well but was more fragile.

[HwAoRrDk]

Aargh! So I finally get around to submitting my stencil order to JLCPCB, and it's a good thing I ticked the "confirm production files" box, because otherwise I would not have realised that not only have they modified my stencil design, but also chosen a different stencil thickness than I was counting on - 0.12mm versus my assumption of 0.15mm (which is what all previous stencils I've had from them were).

All this fretting about aperture sizes to get things just right and they throw it out the window anyway! They modified only the apertures for a QFN and FFC footprint (both 0.5mm pitch), changing the shape and size. They made them with rounded ends, and narrowed the aperture slightly for the QFN (0.26 vs 0.24). They also segmented my QFN's centre pad aperture for some reason - not sure why, the original is not excessive size, only 42% area of pad.



Footprint for QFN from my original gerber on left, JLCPCB's modification on right.

What should I do? Accept their changes under the assumption that they know what they're doing, or tell them to leave it as-submitted and make the stencil 0.15mm thickness instead of 0.12mm?

[SMTech]

Most of our stencils with 0.5mm pitch QFNs are 0.12mm and I find that works well - This little table here would tend to agree https://www.7pcb.com/blog/stencil-thickness-calculations.

The board I am working on today is 0.4mm pitch UQFN with a 0.12mm stencil, it needs inspection and underwipe to spot and prevent blockages on that device.

I doubt the QFN alterations are a problem, quartering your centre pad seems unnecessary but rounded corners are a good thing as paste sticks in squarer ones.

[HwAoRrDk]

Most of our stencils with 0.5mm pitch QFNs are 0.12mm and I find that works well - This little table here would tend to agree https://www.7pcb.com/blog/stencil-thickness-calculations.

I don't know where they sourced their table from in that link, but the actual IPC-7525A says that for 0.5mm pitch QFP/QFN a stencil thickness of anywhere from 0.125 to 0.15mm is suggested, whereas they say that 0.15 is only suitable for pitch >0.5mm.

I doubt the QFN alterations are a problem, quartering your centre pad seems unnecessary but rounded corners are a good thing as paste sticks in squarer ones.

The corners on all my pads are rounded (not sure if it is clear in the screenshot), but surely there is a point of diminishing returns for a shape such as JLCPCB have done (circular ends)?

I worked out the area of the segmented centre pad, and it lowers it from 42% to 36%. I really can't envision why they did that. Is it because they think that area is too big and will have too much solder paste? Or perhaps because I actually have a via in the centre that is still covered by the paste (the castellated shape of the aperture is to avoid the 8 other vias, but obviously you can't have an island in the middle of an aperture for the 9th), and they felt it should be uncovered? Or maybe they just a have an automated CAM rule that says "aperture rectangle area >N, segment it".

I tried asking their online chat support why these kinds of changes are made, but all I got was "our engineer uses experience to best adjust stencil for manufacturing".

Maybe I should just reject their modifications and ask for as originally submitted with 0.15mm thickness. After all, that was the expectation I originally had going in to the stencil order... But I dunno, I'm still torn.

[temperance]

What should I do? Accept their changes under the assumption that they know what they're doing, or tell them to leave it as-submitted and make the stencil 0.15mm thickness instead of 0.12mm?

Those apertures are unacceptable because the convex corners might lift while printing.

[HwAoRrDk]

Those apertures are unacceptable because the convex corners might lift while printing.

Which are you referring to?

[SMTech]

Ahh yes, you have little unsupported tabs sticking out into your paste area, these can snag on your blade, JLC have fixed this by adding a support strut. Arguably what they should have done is change the whole thing to four simple squares instead to keep your ratio.

I would argue that even with IPC rules 0.5mm is right on the borderline, I find 0.12 thickness work best for me, I am printing manually despite running volumes that probably suggest I should not (my eyes concur). It is possible if was running an automatic printer with its better tolerances in all axes and measured angles and pressures 0.15 might be more successful for me than it is now. So also would higher volumes inferring fresher paste and better climate control, we can't have everything.

[temperance]

The correct method is to use small rectangles or squares.

Taking the guesswork out of it:

Those pad's usually require via's. I usually make or request the distance between those apertures to be made wider than the via drill size. The via's are of course located underneath the bridges between the apertures. My idea is to prevent solder wicking because surface tension keeps the molten paste from flowing into the via's. Some wicking can't be avoided. But it is much less if the via's are free from the start.

[HwAoRrDk]

Sigh. I decided to sleep on it and decide what to do today. But JLCPCB auto-confirm production files after 24h! So I guess I'm getting the stencil with their modifications whether I like it or not now...

A 24h period is too short, especially with time zone differences, etc. What if you wanted feedback from other people, and they weren't immediately available? I mean, I get that they don't want things sitting around in limbo forever, but 24h is too short. 48h would be more realistic.

Ahh yes, you have little unsupported tabs sticking out into your paste area, these can snag on your blade, JLC have fixed this by adding a support strut.

Ohh, yeah, I never thought of it like that. Well, I haven't personally had any problems doing aperture shapes like that before. I'll reconsider for future.

[Matt-Brown]

The stencil mod to the wfn is also to allow an escape path for air. It also allows the qfn to center better. They windowpaned it which is what I would have asked for. As solder melts it will bead up in the center (like a bubble) and the windowpane makes smaller equal beads.