I got a message from PCBWay telling me that the gaps between my pads for a USB C connector were too small for their black or matte black solder mask and I could remove the mark or make the pads spacing 0.22mm.
As all the ICs and headers have a 0.2mm spacing on my board, made even smaller by the 2mil solder mask expansion for a total gap of 0.0984mm there is no chance of making that gap 0.22mm.
So that leaves bare FR4 between the pins, how terrible is that going to be for reflowing? (planning on using a hot plate to flow some 180c paste).
I’m writing from home - I don’t have links at hand.
I think each IC manufacturer have at least one app note about this subject.
The mask offset can’t be smaller than say 3 mils because of production tolerances (if, because of tolerances solder mask will come on the pad border then IC can have a problems to position correctly.
The mask strap between pads should not be thinner than say 3 mils because then it may break away and during following processes it can stick elsewhere at the PCB being a problem for something.
So when you are not able to ensure minimum offset and minimum mask width you should make one big mask opening for a row of pads.
More then 10 years ago I have done first time such opening for the 0.4mm raster IC. Then I had a series of neighboring pads connected together. I connected them with the track going directly between their centers. After reflow soldering thin left between them looking ugly (everything was working correctly). I was told by contract manufacturer who assembled our PCBs that I should not connect them directly but with track going first to the out direction (or in). After I corrected it there were no ugly looking PCBs even there were no mask between pads. That IC was 100 pin TQFP 0.4mm.
At my current PCB I have 0.4mm raster IC that I have a solder mask between pads but it was after I asked contract manufacturer and he asked PCB manufacturer if it can be done. But at the same PCB I have other IC that I have no solder mask between its pads.
It’s probably just fine.
When IC pin pitch gets too narrow, there is just no room left for solder mask in between.
And solder does not stick to the PCB itself and the lack of solder mask will not influence the chance of solder bridges. Even if there were solder mask between the pads, the pads will still have to be exposed to be able to solder to them.
The amount of solder on the pads is quite critical. Too much solder will increase the chance of solder bridges significantly.
I just had an Idea, but I don’t know if it will work. You can use relatively long pads, and then use a smaller cutout for the stencil. The Idea is that the longer (and exposed) pad can wick a bit of solder away from the connection if needed, so the total amount of paste on the PCB is less critical. Longer pads also help with rework if there are bridges. Do not though, that it’s just an Idea, and I’m no soldering expert.
Being absolutely not expert in this subject I think that ICs are not placed perfectly and they position themselves during reflow. I think that if IC pins are moving toward pad ends at one IC side than surface tension force at this side lovers (changed the direction from horizontal more to vertical) while at the opposite side increases. Making these forces equal positions the IC.
If the pads will be long I would be not sure if forces changes will be enough to position IC correctly. Changes in position will make very little force differences. May be the pads on both other sides will help in that situation.
There are two options to adjust the amount of paste on the board - the thickness of the stencil and the size of the aperture. The thickness is selected according to the smallest component or pitch … If you are not experienced, you can refer to the datasheet for your components, the thickness is usually indicated there … in more cases, the size of the aperture in the stencil is -0.1 mm from the size of the footprint
Keep in mind that if you do not apply solder mask on the footprint it will result in all traces being exposed, so you can run into issues like solder bridges between pads and traces.
Also: if you go with green solder mask you probably will be able to fit solder mask slivers between the pads. Green solder mask is mechanically more robust and thus can be applied thinner.
I agree that solder bridges are easier to spot then connections starved of solder. Especially because faults due to not enough solder may lead to intermittent contact and can be very hard to diagnose.
This thread was also started specifically for an USB-C connector. The pitch of those connectors can be very small, and the contacts can also very difficult to access for inspection and rework. I recommend you compare a bunch of connectors and keep this in mind during the design of the PCB.
I’ve been here - 56 pin QFN with 0.4mm pads spacing and 0.2mm pads.
Just put a solder mask free area along all the pads on each side, but backed off the length of the aperture on my solder screen for the pads.
No bridging!
It’s more forgiving with paste alignment with solder mask between pads, but if you can get that bit right and not over do the amount of paste, you’ll be fine.
I was building thousands of my circuits like this and it was very rare I had bridges. If I did, it was because of poor paste alignment.
Similarly, I’m often in the position of ending up with no solder mask between pins on fine pitch parts. So long as your solder stencil is good and your process control is good you should have no issues. We do this on production boards all the time (>10,000 pieces).
It sounds as though this is a single/low volume pcb, so if you do end up having to remove a few bridges its not really a big deal. A bit of flux, some skinny solder wick, and you’re golden. If you don’t want to remove too much solder, use wick that you’ve already partly loaded with solder.
I don’t think this is going to be an issue. Even some chip manufacturers have this in their datasheets. I use to do that with all small pitch components and we don’t remember having any particular issues with the yield.
