Ignore missing connection?

[hitachii]

Hello, this is my first post, regarding my first PCB!

For my project, I will be doing an at-home PCB etching using one-sided copper-clad laminate. My project involves using two separate boards that are connected using stackable pin headers. I have made my PCB layout for both boards, using only one schematic/PCB file, placing both boards side by side, separated by edge-cut.

Since I’m using single-sided copper-clad laminate, I’ve had to create some points where I’ll have to use a jumper cable, so I’ve added a few connector holes to do so. For all of the places using a jumper on the same board, I’ve been satisfying the DRC by simply routing tracks using B.Cu.

The problem is that I cannot use this method to connect the stackable pins because the tracks are, naturally, blocked by the edge cut. Is there a way to ignore the missing connections in the DRC? Is there a better method for this (aside from starting over with one PCB per project, hopefully)?

Thank you, I’ve been enjoying using KiCad very much.

[retiredfeline]

You could just ignore those messages since you know what’s happening.

[hitachii]

True. There are quite a few so my primary concern was missing a flag that was not intentionally there. I guess it’s a good exercise in diligence though!

[hitachii]

It has just occurred to me that this would be an effective use of local and hierarchical labels! Problem solved!

[paulvdh]

One way of doing this is to define your PCB as a dual layer PCB.

Then the bottom layer would be just as it is now, and you use the top layer exclusively for wire jumpers.
Then also adjust your via sizes (hole and diameter) to something that satisfies your needs to solder wires to these pads.

---

Another approach is to treat these wire jumpers as real PCB parts. This means making them a part of the schematic and defining footprints for them.

[hitachii]

@paulvdh

Another approach is to treat these wire jumpers as real PCB parts. This means making them a part of the schematic and defining footprints for them.

I like this approach! Is there anything in the library which is similar to an arbitrary length wire, like a physical 22 awg wire or similar?

[paulvdh]

They are probably not in the default KiCad libraries, but I do know that Blackcoffee has some expertise in this area.

For example, he posted a library of such wires in the post below:

Jumper Wires for Single/Double Sided PCB's

I CNC mill more Single-Sided PCB’s than I care to admit and, when possible, I prefer using Jumper-Wires in lieu of making Double-Sided boards. Graphic layouts can be helpful and, having No effect on circuits or PCB manufacture, jumpers can overlay on top of Ratsnest lines (in PCB layout) thus adding a missing link to layout concepts. Attached zip file contains several Jumper-Wire footprints (.mod and Step files) for PCB: 8mm, 12mm 20mm 25mm, 30mm, 50mm The File: JumperWires.zip (141.7 KB) •…

(And in some other threads also. He does quite a lot of stuff by combining KiCad and FreeCAD).

Making A Jumper Wire - Video

Finishing up a Single-Sided PCB project, I needed a 50mm jumper wire. Figured I may as well make a Video. This Video uses FreeCAD v18 with Two Bodies - all made in the PartDesign Workbench. It’s Exported from StepUp Workbench. Both the WRL and STEP are usable as exported. Making; a wire, a harness, cables, etc. is all so similar The YouTube Video is posted Here Screenshot below [Screen Shot 2020-04-23 at 3.03.57 PM]

[BlackCoffee]

Screenshot below show some thrown-together examples; I drew some graphics to represent Jumper-Wires and dropped a Jumper-Wire footprint and other footprints onto PCB without any thought or hookup’s - just to give you the idea of possibilities…

If PCB’s are on the same Plane, you can draw them in Edge_Cut layer and connect them with a Jumper-Wire or just a Graphic representation on a desired layer (as shown).

If PCB’s are at different Plane elevations, you can make footprints of them and set their ‘Z’ dimensions to desired height and use jumper wire or make you own wires.

Easy to do for those with some CAD experience, otherwise, it’s a good education and perhaps useful for other purposes…

EDIT: Added info re ‘Stackable’ ability…. Last screenshot
If you have both PCB’s in the same Project…
PCB1 has Pin Socket
PCB2 has Pin Header

• Save a Copy of the PCB file (can save in the same Project folder) Name it PCB2
(for clarity, name the original as PCB1)

• Delete PCB2 from PCB1
• Delete PCB1 from PCB2
• In PCB2, Export it as STEP
• Make a Footprint and use PCB2 Step file for the 3D model.
Offset it’s ‘Z’ dimension for desired height.
• Place the new Footprint (of PCB2) into PCB1 and position as desired.

Screenshots…

Two PCB’s Pin_Header and Pin_Socket