Friday, July 21, 2017


That beautiful purple board I received yesterday won't work. If it had been stuffed and plugged in, it would have immediately shorted out anything plugged into it.

One of the features on the board is a super-wide (for a 6-mil PCB) strap between the two adjacent 5V pins coming from the Pi. When I had a close look at it, I saw a thin little gold crescent around part of the hole. It took a little bit for it to dawn on me that this was the ground plane, which was visible through the mask, plated in gold, and not protected from shorting with the other contacts:
 The effect is everywhere on the board. I saw it first on the strap in the upper-left, but this magnified version shows it on the motor power section and connection to the Arduino. Note the crescents around the top of D3~ and RST, and the slivers of ground plane visible through the mask around the isolator footprint.

I don't think that there is anything that can be done to fix it. I also don't think that the encoder board is affected, so at least I can still use that. I'll try to stuff it, but I will check continuity closely. If any of the solder bridges the 6mil gap, then the short will exist.

I'm pretty sure the problem comes from settings in the ground plane. Since OSHPark can make 6mil boards, I take full advantage of the feature. Unfortunately, this interacts with a bad default in Kicad. Fortunately, that is easy to change, but it would have been nice to know fifteen dollars and two week ago. The money isn't a big deal, it's the time.

Kicad was even trying to tell me that something bad was about to happen. Not from the DRC (although that would have been nice) but in the images. Here is the old, bad design:

The purple rings around the pads are the soldermask gap. You can see a slight red tinge around the edge where the mask gap overlaps the ground plane.
The OpenGL preview shows it too, perhaps in an easier-to-understand form.

To fix it, use the Dimensions/Pads Mask Clearance menu option

Change the Solder mask clearance value from its default... (Yes, I design my boards in US units. You got a problem with that?)

Change it to zero.

The borders of all the pads are now black, indicating the solder mask gap doesn't span the space between the pad and the ground plane

 This option has settings in several places: The global setting I talk about above, the zone setting (which I haven't found), the footprint setting, and the individual pad setting. The later settings in the list have priority over the earlier ones, but the earlier ones are used as defaults.

In general with modern fab processes, you should set this value to zero. This will describe a hole in the solder mask the exact size of the pad. The fab can and will edit this to match their process, so don't worry about getting it too small.

Thanks to a YouTube video by My 2uF for help finding this setting.

No comments:

Post a Comment