I’ve got a board ready to send off to Oshpark, that has a micro-USB port with plated slots (oval pads). There’s quite a bit of discussion already on how to do the callouts since Oshpark doesn’t support the default KiCad callout (G85 drill drag), and I’ve referenced the following pages:
The problem I’m having is that when I use one of the accepted callouts (drawing a boundary or drawing a path with the slot width on Edge.Cuts), my ground plane zone no longer connects to the pad like it did before I added the slot callouts. I’m also unable to connect a trace to the pad. This makes sense because of the DRC rules, but poses a problem for me.
Here’s a picture of the problem with one of each callout type, where I’ve changed the Edge.Cuts layer to orange for visibility:
Smart. I drew the callout on the Eco1.User layer, then merged the Gerber file for that layer with the one for the Edge.Cuts layer. Couldn’t (quickly) find a way to do it with gerbv or KiCad’s viewer, but it wasn’t very hard to do by hand then verify the results with gerbv. Looks like gerbmerge could be a potential option in the future. Looks like it worked well with Oshpark’s system, got the board ordered so we’ll see how it turns out!
This must have been the case in the past already. Otherwise the old workaround of placing edge cut drawings inside the pad would not have worked. (That was after all the way they documented it on their webside. See the oshpark link in the first post.)
The new thing is that you would no longer need to rely on this workaround as they now can read kicad oval drill definitions directly. (You can now change the pads drill shape to oval and remove the edge cuts drawing)
I thought that was the aim of making a slot inside of a pad. Otherwise it would not make sense to do it that way. (It is even documented that way in the oshpark link provided above. So it seems this was the case even before their recent changes to how they handle kicad slot callouts)
KiCad has separate tag for NPTH, so you should be able to create a non-plated slot, via the NPTH file, if you really want to.
I would guess any board FAB that can manage a slot, does not care if it is pre or post plating - they just load the drill files for each state, where they exist.
It was a long conversation. I’m pretty sure Laen changed their software to detect edge cuts that cut copper on both sides. It’s fairly new. The fab guys asked for it because they had to do it manually.
Some manufacturers may interpret routed slots where copper surrounds them and touches them as plated, and where they don’t touch copper as non-plated. I don’t know what’s the case with oshpark.
Adding my recent experience here. I too am using OSH Park to produce some boards that have slots in them, though I think the problems discussed here are largely PCB fabricator independent. I need some high voltage isolation slots, and therefore they must be non plated in nature. After some back and forth email with OSH Park, I have opted to put the slots on the edge cuts layer, using lines of appropriate router bit width. This produces the type of gerber files needed by OSH Park, however unfortunately it partially breaks Kicad, as it gets upset with open ended lines (IE non closed loops such as a board edge) on the board.
It will be really good to see Kicad better manage the creation of slots in future, and I personally think they should be on the edge cuts layer, but that’s just my personal opinion and somebody else may have a better idea. Should anybody wish to see the email trail for more information, please just shout.
