How can I design this THT footprint?

[PartialDischarge]

I don't know how to design this footprint for a panel BNC connector. The custom shape primitives seem to apply to the exterior of the footprint not the interior hole.

On the outside it is circular 12mm in diameter, and on the inside it is 9,6mm but with a slot as in the picture.

[shapirus]

Not sure what you are trying to achieve. This is not a THT part, it's a panel mount connector. Do you want to mount it on the PCB somehow?

If you want to create a cutout shaped like what is shown in the drawing, then you can simply draw it using an arc and a line in the edge cuts layer. Then add an outer circle in the courtyard layer, if necessary.

[PartialDischarge]

Not sure what you are trying to achieve. This is not a THT part, it's a panel mount connector. Do you want to mount it on the PCB somehow?

Exactly, its a PCB in which the connector will be mounted on one side with components on the other. The slot is important as this is what prevents rotation

If you want to create a cutout shaped like what is shown in the drawing, then you can simply draw it using an arc and a line in the edge cuts layer. Then add an outer circle in the courtyard layer, if necessary.

I know how to create a cutout like that, but that would not have a THT connection with metal on both sides of the PCB to make contact with the connector, ie I'm trying to avoid the solder on the tab of the connector and have a direct connector to board contact.

Maybe its my bad for trying to do this as someone can argue that I should solder the tab to a cable and then the cable to the board but that is just a waste of time

[golden_labels]

I’d like to point out that it’s a panel mount connector, as shapirus noted, not a part going to a PCB. Not sure, how you’re trying to connect it to a PCB, in particular without solder, how do you want to provide robust support and avoid stresses. Not even sure, what part of it is supposed to touch copper on the PCB.

Can you draw a PCB position on that picture, which you provided earlier? Touching both connections, marking which copper goes where?

[PartialDischarge]

I’d like to point out that it’s a panel mount connector, as shapirus noted, not a part going to a PCB. Not sure, how you’re trying to connect it to a PCB, in particular without solder, how do you want to provide robust support and avoid stresses. Not even sure, what part of it is supposed to touch copper on the PCB.

There is nothing preventing a panel connector to be mounted in a PCB. Actually it will go thru 2x1,6mm FR4 boards which is more than enough for strength.
Apart from this discussion of whether this connector is or not a THT part, the question is still if Kicad can do an arbitrary internal cut with thru hole plating.

Can you draw a PCB position on that picture, which you provided earlier? Touching both connections, marking which copper goes where?

Only the ground will connect directly to the PCB, the other central pin of the BNC needs a cable of course.

[Doctorandus_P]

You would have gotten much better answers if you asked the right answer.

The answer "it's not for PCB mounting" is a good answer to your original question.

But for your later question. Plating the side of a non-round hole is more of a production problem then of the software you use. Plating for such holes falls under the chapter of Edge Plating and that is a bit of a non standard thing. As far as I know you have to contact your manufacturer on whether they can do it for you, and on how they want it specified. Some want this on a separate drawing (You could use one of the user layers in KiCad for this).

But I would not bother with this. I would just use a bunch of via's to stitch the pads on top and bottom together. Any PCB manufacturer supports this, there are no extra costs or delays or miscommunication, and it's probably "good enough" for any signal that is able to pass through a BNC connector anyway.

[shapirus]

the question is still if Kicad can do an arbitrary internal cut with thru hole plating.

Ah, now, that's the right way of phrasing the question :).

Nope, it looks like this is yet another real life scenario feature missing in kicad. Any plated hole or slot apparently must be a pad, and pads can only have a few predefined shapes. There is some pad editing mode called "Edit pad as graphic shapes" in the context menu (right click a pad in the footprint editor), but it doesn't seem to offer anything useful. At most, it seems that you can only move the sides of the pad if it's rectangular, that's it. Can't select the hole, can't draw anything new. Maybe I'm missing something more or less obvious there?

p.s. someone tried to do this before: https://forum.kicad.info/t/custom-shape-th-footprint/25859/11
as usual, hard to understand if it's still applicable because of all the changes in the UI.

[shapirus]

Plating for such holes falls under the chapter of Edge Plating and that is a bit of a non standard thing.

Don't all slots and holes get plated by default unless they are covered?

On the other hand, it's a question of whether the slots/holes are milled/drilled before or after the plating process. If we take jlcpcb as an example, they support oval plated slots (without specifying any size limits, it seems), but they must be designated as pads, and anything not circular has to be milled. So apparently milling takes place twice, the second time after the board is finished, when the mouse bite tabs etc. are made?

[shapirus]

But I would not bother with this. I would just use a bunch of via's to stitch the pads on top and bottom together. Any PCB manufacturer supports this, there are no extra costs or delays or miscommunication, and it's probably "good enough" for any signal that is able to pass through a BNC connector anyway.

Besides, that copper on both sides will also be joined via the connector's body itself when the nut is tightened. And no extra work in kicad for that.

However, the question of how to create a pad of an arbitrary shape in kicad is still valid on its own. Does anyone know how to actually make use of the "edit pad as graphic shapes" function?

update: ok, it's easy to add copper by drawing it on the F.Cu layer, but still not clear how to make custom shaped holes in THT pads and whether it's even possible.

[gamalot]

Like this.

[shapirus]

Like this.

That's how it'll actually be milled. But how do we make this shape a hole in a plated THT pad in kicad?

[PartialDischarge]

p.s. someone tried to do this before: https://forum.kicad.info/t/custom-shape-th-footprint/25859/11
as usual, hard to understand if it's still applicable because of all the changes in the UI.

Exactly that's something quite similar to what I'm trying to do. I'll read that thread...

[shapirus]

Exactly that's something quite similar to what I'm trying to do. I'll read that thread...

Let us know what you end up with. That's not an unusual task, yet quite unclear as to how to do it in kicad.

[golden_labels]

Oh, and now this is a clearer question!

Assuming you want the inside of the cutout to be plated: you can’t. At least not reliably. While you probably could hack around to create something looking right in software, the PCB manufacturer wouldn’t produce it or the results may differ from what you expected.

The problem is, that files you send to the manufacturer describe PCB surfaces only. Their software also takes only that into account. Cutouts and drillhole positions (even plated) are also just flat drawings on these surfaces. Edge plating (this is the keyword you search for) requires separate process, completely incompatible with basic workflow.

If your manufacturer offers edge plating, talk to them. They will tell you, how to mark the edges. Here is an example from JLCPCB.

[Doctorandus_P]

I had a look at the Gerber X2 standard.

Apparently there is a .FileFunction  for Plated routing. It's also possible to specify a depth (between which layers) or PTH.

Plated,i,j,(PTH|Blind|Buried) [,<label>]

Plated drill/rout data, span from copper layer i to layer j. The from/to order is not significant. The (PTH|Blind|Buried) field is mandatory. The label is optional. If present it must take one of the following values: Drill, Rout or Mixed


But as far as I know, there is no direct support in KiCad. I guess you can draw it on a user layer, and then modify the .FileFunction with a text editor, but this is clearly not optimal. I also have doubts about general support of the more exotic features of the Gerber format by PCB manufacturers.

[PartialDischarge]

Assuming you want the inside of the cutout to be plated: you can’t. At least not reliably. While you probably could hack around to create something looking right in software, the PCB manufacturer wouldn’t produce it or the results may differ from what you expected.

The problem is, that files you send to the manufacturer describe PCB surfaces only. Their software also takes only that into account. Cutouts and drillhole positions (even plated) are also just flat drawings on these surfaces. Edge plating (this is the keyword you search for) requires separate process, completely incompatible with basic workflow.

If your manufacturer offers edge plating, talk to them. They will tell you, how to mark the edges. Here is an example from JLCPCB.

That does not make any sense because hole plating is a chemical process not a mechanical one, the process will not care if the hole is circular or not. And this is not the same as edge plating

[forrestc]

That does not make any sense because hole plating is a chemical process not a mechanical one, the process will not care if the hole is circular or not. And this is not the same as edge plating

I think the issue here is that for a certain size and shape of the hole, it isn't uncommon for the process to have to be done during a milling step.  Milling often comes after the plating step. I.E., All the holes are drilled, the board is plated, etched, solder mask, silkscreen, and surface finishing added, and only then is milling done.

If you have holes that need to be plated that are incompatible with the drilling machinery, you either have to add a milling step before plating or a plating step after milling. I suspect the confusion here is that the "plating step after milling" is when edge plating would occur so some people call it 'edge plating' if it gets done at that step.   Note that all of the above is manufacturer-specific so what can be plated without additional cost/steps is going to vary depending on who you get to make boards.  Even my low-cost manufacturer can do 'elongated holes' up to a certain dimension, but they can't do anything more than that if you want it plated.

For the original poster's application, I'd probably just not worry about having the hole plated.  Put a pad top and bottom and make sure that I had enough vias such that the circuit itself wasn't depending on the connector making the connection from top to bottom.   Part of the reason why I would do this is that I know that a plated mounting hole on a multilayer board is just asking for problems, as the mounting screw can cause various types of damage which is worse with a plated hole (such as fod, or cracked barrels, etc).   So, for mounting holes that need to be connected to the chassis through the screw, generally, the hole itself isn't plated.  Instead, a ring of vias is placed around the hole with copper being on top and bottom of the board - but no plated barrel in the hole.   Ideally the vias would be outside the screw head area to prevent them from being damaged as well.

For the OP, mounting the connectors through the board will result in similar pressures/potential damages as you would see with a mounting hole which is why I'd just do the same thing as I'd do for a grounded mounting hole.

[PartialDischarge]

Realistically speaking the thru hole plating is not really necessary since the component is not going to be soldered. So I'll probably end up with using an edge cut with two copper layers on each side joined by vias.

[Silenos]

I did once a round 8 mm diameter hole in a PCB, accidentally had it plated and all I got were the complaints from factory that they cannot manufacture that. The plating had to be removed.
For this specfic part: I don't think you need side walls plating at all, or on the board surface either, and still I would not do that as the contact seems unreliable due to the corrosion and nut loosening over time. Such parts are either designed to connect to perpendicular board behind the panel, or just only through soldered flex wires. The "flap" with a hole is gnd/coax signal I guess.

[golden_labels]

One may draw whatever they want in a CAD program. Doesn’t mean anybody is willing or even able to produce that. Blueprints must match existing and offered manufacturing processes.

Manufacturing processes are designed and optimized to produce specific features, not arbitrary things the customer may imagine. One of the steps is producing plated drillholes. This is done with tooling for making only circular holes of small diameter.⁽¹⁾ I can put a 50 mm diameter hole in a gerber file, but do you think they have a 50 mm drill bit in the CNC machine? After the holes are drilled, plating is applied before continuing to next steps.

Making arbitrarily-shaped cutouts is done at the opposite end of the process. Long after holes have been plated. After cuts are made another step may be added to plate them. But this is a step completely separate from hole plating, you must pay for it extra, not every manufacturer offers it, and there is no standard way to mark it in gerber files. You contact your PCB etching company and they tell you, what can be done and how to mark edges for plating.

⁽¹⁾ Recently you can get more shapes, but they are still not arbitrary, expected to be small, and require an additional step (hence you pay more $$$). Historically you could also get some other shapes, but that was done as cutouts and didn’t offer plating.

[PartialDischarge]

I can put a 50 mm diameter hole in a gerber file, but do you think they have a 50 mm drill bit in the CNC machine? After the holes are drilled, plating is applied before continuing to next steps.

I actually believe many holes are not drilled but milled, since your argument can be applied to small diameters, do they have 5.25mm drills? and 3.42mm? No but they do these holes and pretty accurately, so that's why I believe (*) many holes you think are drilled are milled in reality.

* Unless they round to the 0.1mm and have all drills in 0.1mm steps....

[shapirus]

I actually believe many holes are not drilled but milled, since your argument can be applied to small diameters, do they have 5.25mm drills? and 3.42mm? No but they do these holes and pretty accurately, so that's why I believe (*) many holes you think are drilled are milled in reality.

* Unless they round to the 0.1mm and have all drills in 0.1mm steps....

Also, plated oval slots seem to be pretty standard (no added cost).

[golden_labels]

PartialDischarge: I’m helping you. What’s your goal in trying to argue? If you already know all the answers, why did you ask in the first place? This is not how this works.

Forgive me for providing you with the big picture, so you could get the general gripe on the issue and get this done, instead of writing you a 5-tome book covering all the possible variation in the process, all the details, all the exceptions and exceptions to exceptions, and another 20-tome book of auxiliary knowledge needed to understand why some things are not done in reality despite being technically possible. Most notably I beg forgiveness for using a footnote instead of 24 pt bold and blinking font, so you wouldn’t miss the glimpse of such variations. /s

If you want to know, why the process of using a 1.0 mm drill to make a 1.04 mm hole doesn’t scale to your cutout (or requires additional steps or specific fabrication process to be available), you already have access to the internet. You can find the information. I’m done with it.

[forrestc]

* Unless they round to the 0.1mm and have all drills in 0.1mm steps....

I'm pretty certain that's what some do.  It's not uncommon to see a hole size spec of +-0.1mm or thereabouts.   JLCPCB is +0.13 -0.8mm.  Advance circuits seems to be +-0.762 (3 mils). 

[PartialDischarge]

* Unless they round to the 0.1mm and have all drills in 0.1mm steps....

I'm pretty certain that's what some do.  It's not uncommon to see a hole size spec of +-0.1mm or thereabouts.   JLCPCB is +0.13 -0.8mm.  Advance circuits seems to be +-0.762 (3 mils).

And there is a high chance that is correct, 0.1mm drill sets are widely available. However, how do they do slotted plated holes? by multiple holes or by milling?

At this point I think the real challenge is defining this type of pad in software not in the manufacture