2
\$\begingroup\$

After designing a board in Kicad with an SMT32L0 on it, I sent it to seeedStudio and when I received it, I noticed that some of the pads on the stm32 are missing soldermask: enter image description here

I checked the gerber file for the soldermask and there is no apparent hole in the stm32 pads : enter image description here enter image description here

I noticed that the pads missing the soldermask are tied together, but in two place there is also a pad that is not tied to the rest of the group that is missing soldermask which makes this impossible to solder by hand.

Upon inspection with a microscope, I noticed that the missing areas are all in the same shape which looks like this :

enter image description here

(blue is pads and copper and black is the cutout in the soldermask)

What happened with my pcb?

Here is the back soldermask layer with a gerber viewer : enter image description here

with the back copper : enter image description here

\$\endgroup\$
  • 1
    \$\begingroup\$ Did you receive just one board or are there multiple board with exactly the same problem locations? Some background- for the really fine pitch components, a lot of board houses just don't have the process control down well enough, especially for small runs with particular technologies (there are many soldermask application systems, not all are equal in resolution nor $). The house should have a standard spec sheet describing what their capabilities are. In practice for packages like TSSOP you rely on the paste stencil to get the solder meniscus to form properly with rework at inspection. \$\endgroup\$ – isdi Oct 22 '18 at 22:05
  • 2
    \$\begingroup\$ The proof is in the gerber files; not the KiCAD design files. If the gerber file is correct, then this is a seeedStudio problem. If you haven't already, view your gerbers with a third-party viewer such as gerbv (free). Ensure that your source files actually are correct, then give seeedStudio a call. It may be that they are unable to do what you want, but they may have simply made a mistake... \$\endgroup\$ – bitsmack Oct 22 '18 at 22:14
  • 1
    \$\begingroup\$ bitsmack is correct, though, no matter what the original KiCAD file indicates, you must go to the Gerber file to see the actual output- that's what the board house will use. To me the KiCAD program indicates no solder dams at all, but given the plethora of design rules that can be incorporated into the Gerber generation, you always need to check those over to be safe. \$\endgroup\$ – isdi Oct 22 '18 at 22:20
  • 3
    \$\begingroup\$ None of your images appear to show any solder mask between the pins. It looks to me as though they've given you more than you asked for. If you were expecting a little strip of solder mask between each pin then your design files are wrong. \$\endgroup\$ – brhans Oct 22 '18 at 22:51
  • 1
    \$\begingroup\$ There's still something odd about that "Gerber view" either the wrong layer set is being used, or there's some suspect intelligent software being used. You shouldn't have labels like that on a Gerber file (pin numbers, netlist, etc.) \$\endgroup\$ – isdi Oct 22 '18 at 22:53
3
\$\begingroup\$

Notice that the images of your soldermask simply show large rectangles which span multiple pins. I'm assuming that this is accurate, although perhaps if you zoom in you would see that they are actually smaller rectangles which just look like they're connected.

Anyway, if they really are large rectangles, this instructs seeedStudio to remove these areas completely. That is, as submitted, none of the pins should have soldermask between them.

It looks like seeedStudio's algorithms added soldermask webbing for you where it seemed appropriate, but the algoritm failed to know your intention for the bridged pins.

I haven't used KiCAD, but either your footprint doesn't have individual mask openings, or the software is set to gang them all together (likely in the Design Rules).

Regardless, these can be soldered with care, so you don't necessarily need to scrap the existing boards...

Good luck :)

\$\endgroup\$
  • 1
    \$\begingroup\$ You are absolutery right! I used a footprint inlcuded with kicad and when I went into the footprint editor I noticed that there is no information on the soldermask in the footprint itself. It all happens in the design rules! Good to know :) Now to hand soldering ... \$\endgroup\$ – AntoineLev Oct 22 '18 at 23:07

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.