Minimum gap for Solder Mask between pads at JLCPCB?

[TimCambridge]

My first JLC/Elecrow board included a QFN48 part. I had the board built at both JLC and Elecrow. JLC were a few days quicker and less expensive (especially after their "introductory" discount). Quality seems to be very similar. But...

Elecrow removed the resist web between the QFN pads, JLC didn't.

JLC have a specification on their site (under "Capabilities") but it doesn't seem to include the minimum resist web.

- Does anyone know the number(s)? Elsewhere I've seen 0.1mm (4 mil) for the resist web, in a 0.2mm (8 mil) pad-to-pad.
- Is there a way to specify that the resist pattern should be preserved?
- Do they "massage" the data on prototypes, but not for production panels?

This must be an issue for BGA boards as well, even with NSMD rules. Or is the advice to not use Elecrow for production boards?

[Edited to reverse Elecrow and JLC. In the first version of this post I had them the wrong way round. And see below for helpful comments from experts.]

[thm_w]

According to this post solder mask sliver <0.18mm: https://www.eevblog.com/forum/manufacture/jlcpcb-lead-time/msg1328072/#msg1328072
But since its a cheap PCB fab you are basically at their mercy, they may change whatever they like to make your board more manufactureable.

What was the soldermask width on your QFN48?

Seems you got lucky with elecrow possibly, as their spec is even higher at 0.3mm: https://www.elecrow.com/wiki/index.php?title=Q%26A_for_PCB_service

[TimCambridge]

What was the soldermask width on your QFN48?

Seems you got lucky with elecrow possibly, as their spec is even higher at 0.3mm: https://www.elecrow.com/wiki/index.php?title=Q%26A_for_PCB_service

The QFN is a 0.5mm pad-to-pad part. I used a standard (!) footprint with 0.25mm pads, so the pad-to-pad gap is 0.25mm. The solder mask width was 0.1mm, with a 0.075 mask-to-pad gap. I expect that narrowing the pads to give a 0.3mm pad-to-pad gap would be OK, but maybe there is a better solution. I've sent a query to JLC, I'll post any reply.

Do Elecrow make their own boards or do they use sub-contractors?

Which PCB houses are the current recommendations at the next rung up from JLCPCB (though I'm impressed by JLC's work)?

[ddavidebor]

PCBway. They never bodged one of my boards, nor production runs :-)

[TimCambridge]

Apologies, I mixed up the boards. It wasn't JLCPCB. We sent the design to two board houses and the best version was JLC, with correctly masked pads.

The helpful JLC support engineer tells me that their rule is: " the smallest solder mask width is 0.1mm , and it needs a 0.2mm pad to pad gap". Coincidentally, that is what we had on one of the QFNs (the other QFN was 0.25mm) and indeed the boards were correctly masked.

The second board house was ...crow. Although their masking was messed up, the general quality of their boards was very good, they soldered OK, and they worked 100%. But the production guys don't like the missing masking and I expect we will end up with JLC.

[mrpackethead]

The real issue is the chemistry of the solder mask. Different mask materials behave differnetly and there is a minimum width so it adheres properly.   the last thing you want is a bit of solder mask moving between manufacture and assmebly.  It could really make your day painful.

Where it is tight, i reduce my pad expansion to 0.05mm to start with.    I really like to be able to have a minium of .18mm width in mask, but will run with .15mm if i have to..    For .5mm pitched pins, the pins are typically 0.2 or so..    Sometimes skinnying down the pads slghtly is a good thing.

[xaxaxa]

Solder mask between pins is NOT necessary for QFN. Solder mask has nothing to do with preventing bridging; its only purpose is to stop solder flowing down the trace and leaving a void. In fact the default footprints for QFN in some PCB design software actually has the solder mask between pins removed because inaccurately placed solder mask can make the footprint non-solderable. That's the same reason manufacturers will enlarge your solder mask openings if they know their accuracy isn't that great.

[mrpackethead]

Solder mask between pins is NOT necessary for QFN. Solder mask has nothing to do with preventing bridging; its only purpose is to stop solder flowing down the trace and leaving a void. In fact the default footprints for QFN in some PCB design software actually has the solder mask between pins removed because inaccurately placed solder mask can make the footprint non-solderable. That's the same reason manufacturers will enlarge your solder mask openings if they know their accuracy isn't that great.

Yes, if your bridging pins, you've got other issues to look at.   It Does help, but is not a requirement.

[D3f1ant]

I think IPC rules also suggest not putting mask between pads for sub 0.5mm pitch parts.

[ar__systems]

Why do you need mask between QFN pins? IME QFN never solder-bridge, even if you try.

In one of prototypes I had to fix layout error and shorting two pins of QFN was the easiest fix. I had to use a short strand of wire in the end, since it just would not bridge no matter what I tried.

[flydrive]

Apologies, I mixed up the boards. It wasn't JLCPCB. We sent the design to two board houses and the best version was JLC, with correctly masked pads.

The helpful JLC support engineer tells me that their rule is: " the smallest solder mask width is 0.1mm , and it needs a 0.2mm pad to pad gap". Coincidentally, that is what we had on one of the QFNs (the other QFN was 0.25mm) and indeed the boards were correctly masked.

The second board house was ...crow. Although their masking was messed up, the general quality of their boards was very good, they soldered OK, and they worked 100%. But the production guys don't like the missing masking and I expect we will end up with JLC.

The actual tolerances a board house can do seem to be shrouded in mystery. I just asked JLCPCB what their pad/solder mask tolerances were and they replied pad->mask = 0.127mm and min width mask = 0.1mm. I find that hard to believe from a shop which can do 3mil traces. If that's actually the case you need 0.127 + 0.1 + 0.127 = 0.354 between pads and at 0.5mm pads that leaves <0.15 for the actual pad. That seems very much at odds with the numbers quoted in this thread.

Elecrow's published numbers are ridiculous, something like 0.2 clearance + 0.2 min width which would make 0.5mm impossible. However I got proper numbers out of their support staff a while ago and it's really 0.075 clearance and 0.15 min solder mask width which makes 0.5mm spacing possible if you stick to 0.2mm pads which is .. ok.

I find it odd that JLCPCB which has better tolerances than Elecrow everywhere else is worse on the pad-to-pad numbers.

How did you send your gerbers in by the way? Elecrow has asked me to remove all the solder mask clearance (ie set it to zero) and they just increase it to their minimum before manufacture. As long as I've left 0.3mm between pads, that's always worked to give me some mask. I do this for QFNs if possible even though if they bridge at all it's usually outside the chip, I find having solder mask is vital for things like USB connectors with 0.5mm pitch footprints as they really do bridge under the component.

[mairo]

...
The helpful JLC support engineer tells me that their rule is: " the smallest solder mask width is 0.1mm , and it needs a 0.2mm pad to pad gap". Coincidentally, that is what we had on one of the QFNs (the other QFN was 0.25mm) and indeed the boards were correctly masked.
...

Just to add something here: these specs are probably for 1oz, or less copper thickness. For thicker copper the solder mask width I think will increase (as is the case with PCBWay). I also found that with PCBWay for example the width specs at 2oz varies (this comes from PCBWay themselves) if you are using immersion gold plating, or the more usual HASL/Pb free HASL, as the two are done in two different lines with different capabilities.

[Kasper]

Apologies, I mixed up the boards. It wasn't JLCPCB. We sent the design to two board houses and the best version was JLC, with correctly masked pads.

Would be nice if you edit your first post to add that correction.

[Kasper]

Why do you need mask between QFN pins? IME QFN never solder-bridge, even if you try.

In one of prototypes I had to fix layout error and shorting two pins of QFN was the easiest fix. I had to use a short strand of wire in the end, since it just would not bridge no matter what I tried.

I just did 10 of those manual bridges with 30AWG on 0.5mm DFN. Didn't try without 30AWG.  I don't trust solder bridges without wires inside. That was prohibited when I worked in avionics.  If solder cracks, that wire can make the difference between having electrical connection or not.

Coincidentally, 1 out of 30 of those came with a solder bridge. That was from expensive Canadian PCB and PCA.  They blamed silkscreen near the DFN, didn't have any under it. Said it can raise the stencil, causing too much paste.  They did not mention soldermask.