PCBWay manufacturing problem

[mfli449]

Hi, I'm a beginner, first I created a test board to see how the ordering and quality process is going with PCBWay. When it arrived I was impressed with the quality, so I immediately ordered the right board that I designed for IoT purposes
The PCBs were accepted, I could see their preview, but a few hours after ordering (production has not started yet), I found that I had to change something in the scheme, there was no problem with that, the chat consultant canceled the order
I corrected the changes (added some capacitors) and ordered again. Unfortunately, this time there was a problem with the verification of the plate, I got a message: "As shown in the pic, we found the distance of the solder mask bridge of black ink is less than 0.22 mm , which is beyond our capability".
I don't understand what the problem is, after all, someone approved it earlier and as you can see in the pictures, the same element was made perfectly before. I have two options to choose from: make it green or expose(?). I don't know what to do, what does it mean to expose? There won't be black paint there or what?

In the attachment I added a test photo of the project, how it was made and the problem that was sent to me (It may not be visible in the picture, but there is a black color between these pads on the finished plate)

[PartialDischarge]

Expose means that they will remove the solder mask which is the usual thing to do. Having such a thin soldermask in between pads is not normal.
Usually smaller details like this are caught by production before it starts and not at the first approval.

[ataradov]

This is very common with PcbWay. They sometimes report that solder mask bridges may be beyond their capability and sometimes just submit for production. It might depend on the mood or work load of that specific person on that specific day. It might also depend on the specific equipment your board gets assigned to.

They don't actually remove them, they manufacture as is and sometimes those bridges hold on, but sometimes they break because of over-etching.

And on your board I don't see any bridges, so they either got removed or just broke off.

One thing you can do to help this is not to specify any additional pull-back for the solder mask from the copper (KiCad will show the message about it, and you can ignore it). Let the fab set whatever they want.

But otherwise, for manual soldering it does not matter. And for mass production, the quality of PcbWay prototype boards is not great anyway. They make them on the cheapest equipment and in the cheapest process possible.

[wraper]

They don't actually remove them, they manufacture as is and sometimes those bridges hold on, but sometimes they break because of over-etching.

Generally they remove them, otherwise you will see spikes on solder resist around the footprint where those bridges broke off, also you may see some random bridges still hold. It's very bad as those bridges can break off and get under SMT component terminals.

[ataradov]

also you may see some random bridges still hold. It's very bad as those bridges can break off and get under SMT component terminals.

And I do see that on some of my boards. I agree, it is not ideal, but it is hard to complain for the price.

[julian1]

Pcbway gives details for minimum solder mask, for their standard process here, (0.22mm for green).
    https://www.pcbway.com/pcb_prototype/PCB_Solder_mask.html

In kicad, you can check and set the the minimum width to match their fabrication capabilities. This allows you to preview in Kicad where solder-mask might be removed, where the space between pins is too narrow.
    File -> Board Setup -> Solder Mask/ Paste -> Minimum web width.

0.25mm, is ok for 0.5mm pitch qfn/ qfp.  But it is too coarse for 0.4mm pitch pins, without going to advanced process.

Alternatively, you can leave the board as is, and just instruct them to remove the mask around the problem area - ie. the usb-c connector.