How to create a pad with a D-Hole shaped hole

[albin]

I want to create a PTH for a BNC connector. I would like the hole to be D-shaped in order for the connector not to be able to rotate.

I could draw the D-shape in Edge.Cuts, but I’m not sure if the PCB manufacturer (JLCPCB) will plate the hole.

It will be a 2-layer PCB, so there’s no inner layers.

How would you do this?

The solution I can think of is a round SMD pad on both top and bottom layer, and a D shaped drawing in Edge.Cuts layer. But I’m not sure if JLCPCB will plate this hole.

Is there a solution where the hole is defined in the generated drill file?

I hereby certify that I am not simply asking someone else to design a footprint for me.

This is an auto-generated message that is in place on the “footprints” section of the KiCad.info forum. If I remove it and ask for a footprint to be designed anyway, I understand that I will be subject to forum members telling me to go design my own footprint or referring me to a 3rd party footprint site.

[jmk]

Start with drawing a circle.
Open the properties and change the width of the circular line. This needs a bit of arithmetic. The total width of the circle needs to be the outside width of the pad and the inside width needs to be the size of the hole, so your original circle diameter needs to be half way between these extremities.

Fill in the bottom part with a graphic polygon.
Place a small SMD pad on the appropriate layer and Edit pad as a Graphic Shape (CTRL + E ) twice.

A picture is worth a thousand words. I placed the polygon on a different layer just for clarity.

[albin]

Thank you! I was thinking about doing something like that. But that doesn’t define the hole? Should I still draw the “hole” as a Edge.Cuts outline?

If so, what difference does it make if I do it like you propose, or a simple pad with D-shaped edge.cuts outline within it?

Like this:

I’m not sure if any of these solutions have will result in the hole being plated when manufactured.

[jmk]

I used edge cuts arc and line for the internal hole. I used the same pad on top and bottom, but there is no through hole plating

[RaptorUK]

@albin

But I’m not sure if JLCPCB will plate this hole.

I think they will, for additional cost . . . I made a pad with a trapezoidal hole and they couldn’t/wouldn’t do it as per a through plated hole, they wanted to treat it similar to castleations and charge more.

[albin]

@jmk

I used edge cuts arc and line for the internal hole. I used the same pad on top and bottom, but there is no through hole plating

Yea, I think that’s the only way to define a hole like this. But it feels like it can go both ways regarding plating.

@RaptorUK

I think they will, for additional cost . . . I made a pad with a trapezoidal hole and they couldn’t/wouldn’t do it as per a through plated hole, they wanted to treat it similar to castleations and charge more.

Seems reasonable! I’ll place an order and see what happens. The will probably contact me and ask for additional payment.

It’s not the end of the world if this doesn’t get plated. I’ll spray the board with vias so that it doesn’t really matter if it’s plated or not.

[albin]

Here’s the result. I’ll send it in later today and see what they say.

[RobK]

@albin

The will probably contact me and ask for additional payment.

They might contact you, but I actually doubt it. This is, after all, nothing more special than a slotted hole, which they have no problems manufacturing.

@albin

see what they say.

You’ll have to wait a bit, though, 'cause of the Lunar New Year

[albin]

My experience is that they always send a email for any little detail that they are not 100% sure about. If I have a square test pad on the PCB that I don’t want solder paste on, they often contact me to make sure that I haven’t forgotten to add that pad to the solder paste layer (when also ordering solder stencil). But we’ll see!

Ah! I forgot about the Lunar New Year! Well, I’m not in a hurry with these pcbs so there shouldn’t be a problem.

[ML9104]

Don’t forget that the milling machine is not able to make sharp inside corners. You’ll need to add a couple of “dogbone” corners to solve this.
See this post:

Layout for track 'fingers' for a 3.96mm / 0.156" PCB edge connector?

Well, you have to think of the machine the manufacturer is using: it’s a vertical drill/mill/engraver, meaning a vertically rotating cutting tool. So how should a rotating tool make a sharp inside corner? Answer: it can’t. A laser cutter can, but that’ll add considereable cost to your PCB. The solution is called “Designing for Manufacturability” (meaning you’re responsible). That is where “dog bones” come in: make inside corners like this: [dogbone] In practice, expect a mill diameter of …

[albin]

@ML9104

Don’t forget that the milling machine is not able to make sharp inside corners. You’ll need to add a couple of “dogbone” corners to solve this.

Thank you for your concern. I considered it, but I don’t think that a small radius on these inner corners will be problem so I’ll take my chances. I only need 10 of these boards, so if I’m wrong I’ll take a wood file and sharpen up the corners.

[electrogas]

Do you absolutely need this type of BNC connector. There are many vertical pcb mount BNC connectors that only need a few through holes to solder the legs. For example:

This is from https://www.digikey.com/en/products/detail/amphenol-rf/031-5329-51RFX/2041813

[albin]

@electrogas

There are many vertical pcb mount BNC connectors that only need a few through holes to solder the legs.

Good point! I don’t know why I was set on using a panel mount connector really. Probably because I will use the panel mount types on other places. I could’ve used one of these.

Well, I already placed the order and it won’t really matter if the hole gets plated or not. I just would’ve preferred it and was curious about solutions in Kicad.

[davidsrsb]

It depends on who is assembling the board. Those PCB mount connectors are not easy to solder without melting the dielectric insulation and the panel type requires hand assembly, but more resistant to handling dry joints