DFN 0.65 mm pitch - ENIG or HASL? - Page 1
Forum section: electronics / general

author: HwAoRrDk
author_rank: Super Contributor
timestamp: January 19, 2024, 03:20:08 am
content: I have a PCB design where everything on the board is pretty broad pitch SMD components (1.27 mm pitch SOIC, 0805, etc), with the exception of one DFN package with a pin pitch of 0.65 mm.Normally when working with such leadless packages, I've always been doing so with multi-layer boards and finer pin pitches, so I've always had ENIG finish boards. But I'm wondering whether in this situation, seeing as the pin pitch is fairly broad (0.65 mm) and only a 2-layer board, I could get away with using HASL finish.Is the relatively uneven surface of HASL finish going to cause problems with soldering a DFN package? Especially considering it has a centre pad.

author: ataradov
author_rank: Super Contributor
timestamp: January 19, 2024, 03:45:14 am
content: HASL is not that uneven. Plus it does not matter, since the component will go on the solder paste, which is way bumpier. And by the time it reflows, there is no difference between the two.I also just looked at a few HASL boards, and the solder level there is below the solder mask. So, if you have those solder mask bridges, your component would not even touch the pads.

author: Psi
author_rank: Super Contributor
timestamp: January 19, 2024, 03:58:26 am
content: Maybe if it was a physically large 100+ pin BGA you might want ENIG for higher yields, but anything small shouldn't care much.At least that is what I've found.Because HASL is bumpy you get a normal distribution of how bad the bumps are. At the extreme end of the distribution it can cause issues and hence lower yields.The larger your chip is and the more pads it needs the worse this gets.

author: luudee
author_rank: Frequent Contributor
timestamp: January 19, 2024, 04:10:37 am
content: Quote from: HwAoRrDk on January 19, 2024, 03:20:08 amMost likely, you will apply solder paste on that footprint, right ?So it won't matter if the surface is not 100% smooth ...Cheers,rudi

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 19, 2024, 04:33:52 am
content: If it's hand soldered, it doesn't really matter.I don't mind HASL for smaller footprints, for the above stated reasons. Larger components, it's more risky, and you're probably doing finer pitch and more pins thereof, in such a design, for which ENIG may be desirable.I'd be more concerned about poor centering from that copper bridge between pads. Better to use thin trace segments to fan out the footprint, then connect to wide trace/pour. In general, solder mask does not align with copper, and this way the pads can be non-soldermask defined (NSMD) with excellent alignment.Tim

author: HwAoRrDk
author_rank: Super Contributor
timestamp: January 19, 2024, 06:08:59 am
content: I guess I'm over-thinking it, and HASL will be okay. My experience is that larger unmasked copper areas sometimes have quite a ripple-y solder finish, but I suppose the centre pad on this part is pretty small, and that's highly unlikely to happen here. It's only a 3x3 mm DFN package, and the centre pad is only 2.4x1.65 mm.Quote from: T3sl4co1l on January 19, 2024, 04:33:52 amMy thinking was that because this is a high current switch (up to 5A), I want to make the middle pairs of in/out pads as low impedance as possible, plus it will aid heatsinking. I didn't think it would matter much regarding self-centering during reflow because of the symmetrical nature, plus perfect alignment won't bethatcritical for 0.65 mm pitch, will it? You think it would be better like as attached?

author: selcuk
author_rank: Frequent Contributor
timestamp: January 19, 2024, 07:28:05 am
content: I'm using 0.35mm pitch QFNs on HASL boards. The important thing is not the board surface, it is the stencil surface. I had problems with etched stencils.For that 8 pin DFN package, I expect issues about solder paste under the center pad. Excessive solder may cause one side to go up a little. The image is a WSON8 footprint in which I reduced the solder paste openings to prevent this. This is for a sensor though, you may need a different design for a power IC.

author: HwAoRrDk
author_rank: Super Contributor
timestamp: January 19, 2024, 08:56:12 am
content: Quote from: selcuk on January 19, 2024, 07:28:05 amThe yellow rectangle within the centre pad is the paste stencil aperture. It's already reduced to about 70% the size of the pad. What with the vias in the pad, I figured it will probably be about right, unless anyone thinks otherwise.

author: Kean
author_rank: Unknown
timestamp: January 19, 2024, 10:32:18 am
content: For a while I was always paying the extra fee for ENIG, especially for prototypes. With some suppliers, I found the HASL application could be a bit inconsistent. I didn't want to be dealing with problems caused by that when testing a new design. Also, ENIG can look particularly nice if you expose gold plated copper on the PCB, such as a ring around the PCB edge with via stitching.But now I use lead free HASL finish on pretty much all of my prototype and production boards. I commonly use 0.5mm pitch DFN and QFN parts with very rare issues. Getting the paste application right makes all the difference. Excessive paste will ruin your day.That said, if I start doing any BGA work, or using expensive FPGA parts, I will be specifying ENIG.I think back to the days when I dispensed paste with a handheld air powered syringe, and wonder how on earth I got things to work. I did a lot of rework as I recall.

author: SMTech
author_rank: Frequent Contributor
timestamp: January 19, 2024, 12:52:45 pm
content: I find with HASL you get enough boards sneaking through where is truly not level or even has a stencil lifting blob (it only needs to be bigger than your reduced aperture after all) to be annoying. The absolute guarantee that ENIG is flat, to me is worth it, that said I have seen 2 boards in the last year where the ENIG from PCBWay was faulty and solder paste balled up on top if it instead of reflowing, luckily neither was showing that behavior on an expensive board/complex location.When pasting manually I also find it much easier to align fine pitch seeing gold through apertures than it is HASL silvery grey.The DFN in question doesn't look like the kind of device that is likely to cause anyone issues regardless of finish or process unless you got really heavy handed with the paste

author: wraper
author_rank: Unknown
timestamp: January 19, 2024, 01:09:04 pm
content: For hand soldering, does not matter. For production, not all HASL PCBs are equal. It can range from absolutely awful bumpy surface to nearly flat.

author: Kean
author_rank: Unknown
timestamp: January 19, 2024, 02:24:49 pm
content: Quote from: SMTech on January 19, 2024, 12:52:45 pmThis is very true. The contrast provided by ENIG definitely makes stencils alignment much easier.Quote from: wraper on January 19, 2024, 01:09:04 pmAgain, this is very true - but I've not really seen any issues with Lead Free HASL from JLCPCB or PCBway. I will inspect new panels when they come in and feel them for smoothness, particularly if using fine pitch parts.I am particularly careful with center pads under larger QFNs, as too much paste there plus the HASL will lead to lifting the part. I've seen this in the past with the PIC24EP256GP204-I/ML (QFN44 8x8) which has a rather large recommended center pad. On my stencils, I will generally use smaller than recommended apertures on the center pad.

author: wraper
author_rank: Unknown
timestamp: January 19, 2024, 03:53:06 pm
content: I've got some awful HASL from JLCPCB in the past with random lumps of solder on some panels, flatness seemed to be OK in more recent orders though.

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: January 19, 2024, 04:38:05 pm
content: if it's a few prototypes, then you can always flatten off lumpy HASL with desolder braid

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 19, 2024, 09:02:55 pm
content: Quote from: HwAoRrDk on January 19, 2024, 06:08:59 amYes, this is what I would do.You can calculate Rth of the spokes. It's negligible in almost all cases. At very high currents, like 20A/device, I'd be more interested in pouring over pads, with some potential fallout from assembly as an acceptable tradeoff. And again, the footprint should be re-tuned for SMD (soldermask defined), further facilitated by tighter precision soldermask (specify LDI or the like).Tim