How do I stitch two boards together so I can split them out later?

I have a single PCB file which includes two “boards” (see screenshot below).

The idea is to have this manufactured as one big board but later split them off (because I want to stack these two one on top of the other).

I’ve never done this kind of thing before so I’m wondering what the best practice is here? What do I need to do in KiCad to make sure I can easily split up the two boards after they’ve been fabricated? Is there some tool to indicate that the two boards are meant to be separated?

Cheers.

search “mousebites” and/or “panel” … I do this all the time :wink:

I have done this a couple of times recently with a V-Score.

  • Butt the boards up right next to each other (no gap)
  • Create separate fill zones on each board (rather than one which bridges the two boards)
  • leave any tracks unconnected that bridge the two boards but in reality are connected via headers (KiCad will list the unconnected pads when you run a design rules check, but that’s fine if you know they are connected elsewhere)
  • Draw the Edge Cuts round the two boards as if it were a single large board (ie no edge cut where the boards join)
  • I use the Eco1.User layer for the V-Score, and draw a single line where the board split is to happen.
  • Output this Eco1.User layer as a separate Gerber when you are preparing the Gerber & Drill files
  • Talk to the Fab plant to make sure they know that this is what it means and, if necessary, rename it to something that makes it clear (I use boardname.V.Score.gbr)

In this example, the V-Score is the vertical green line between the two boards, and you can see one remaining air wire which is actually trying to connect the two ground planes together, though this is achieved elsewhere via pin headers.

I’ve been very pleased with the results, and the boards snap apart really cleanly. Mousebites look a lot more messy (IMHO).

Morph

1 Like

You could always use an extra layer to make the connections between the headers and then just don’t plot that layer. At least then you would get a clean DRC.

1 Like

Or use a proper schematic, that doesn’t connect those net’s in the first place, if you don’t want ghost-DRC-errors :wink:

Also V-grooves are good for straight edges and surely nice, but as soon as you get more complicated shapes they won’t work.

1 Like

Thanks for the V-Groove instructions! I’ll keep that in mind for next time. For now I ended up going with tabs/mouse bites as per the fab’s (macrofab) recommendation. I just sent it out to be fabricated so we’ll see how it turns out in a couple of weeks.

Here’s what it looks like:

@1.21Gigawatts Thanks for the tip, I did indeed do this in my board.

@Joan_Sparky By proper schematic do you mean splitting out the two boards into two completely different schematics? I did split the pins of my schematic into two separate sets (one per board) so most of them don’t need to be connected cross-board. But I couldn’t find an elegant way to do that for VCC/GND, so I had to wire those across the two boards on a hidden layer. Any tips are welcome!

P.S. @Morphology, is that a eurorack module? I’m working on one too!

Sorry, I was actually replying to Morphology. But Joan_Sparky does have a good point, if the schematic correctly showed them as two separate boards then a clean DRC could be achieved without hidden layers.

Nets like VCC and GND would need to be unique between the boards, such as VCC1/VCC2 …

1 Like

Yes, it’s a Eurorack Module, well spotted - part of an expandable set of Sequencer modules I’m designing.

That one adds 4xCV and 4xGates to a master module. Up to 8 of these can be chained together to add a total of 32 x CV and 32 Gates.

It’s all working fine, though I haven’t finished the software yet, so haven’t publicised what I’m doing.

Morph.

yes, point taken, though I’m happy to live with 2 unconnected pads in this instance.

1 Like