How can I design this THT footprint?

[forrestc]

However, how do they do slotted plated holes? by multiple holes or by milling?

I had the same question, was about to post it but I couldn't figure out how to phrase it.

I'm guessing either way its done in the same step as the drilling. It wouldn't surprise me to find they just just same machine with a milling bit.   Or maybe they use combination drill/mill bits.  Or maybe remove much of the material with drills and then use a mill to turn it into a slot.   Would be interesting to find out.

Edit:  I just realized I get  manufacturing files back from my preferred board house.   Maybe I'll throw a couple test slots on the next r&d board I send off in a few days and see what the manufacturing files indicate if it includes that level of detail.

[vk4ffab]

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.

Not sure of your ecad, but I would make the cutout as a normal milling operation, put a surface mount pad around the outside top and bottom and stitch them together because its not a plated cutout. Throw in another pad offset for the center connection to be made with wire. Not ideal, but also not impossible. Because my ecad wont let me make weird through holes like that, slots yes, but not holes like you require, so i would have to work around. You want that stitching anyway to add a little board strength when you bolt her on to stop crushing.

[Doctorandus_P]

The difference between a round hole and a hole with a flat side is also minimal. It is the nut that keeps the connector in it's place. With a round hole the main difference will be a few seconds extra during mounting the connector. This is a nice optimization for bigger production runs, but for small numbers it's not worth thinking about much.

[PartialDischarge]

Not sure of your ecad, but I would make the cutout as a normal milling operation, put a surface mount pad around the outside top and bottom and stitch them together because its not a plated cutout. Throw in another pad offset for the center connection to be made with wire. Not ideal, but also not impossible. Because my ecad wont let me make weird through holes like that, slots yes, but not holes like you require, so i would have to work around. You want that stitching anyway to add a little board strength when you bolt her on to stop crushing.

Yes that's what I'll end up doing for simplicity

[PartialDischarge]

The difference between a round hole and a hole with a flat side is also minimal. It is the nut that keeps the connector in it's place.

Absolutely not the case, the slot is 100% needed. Whatever force you tighten the nut with, the BNC will rotate quite easily as you connect/disconnect the male BNC. Believe me I have tried this many times and in different materials.

[Doctorandus_P]

Absolutely not the case, the slot is 100% needed. Whatever force you tighten the nut with, the BNC will rotate quite easily as you connect/disconnect the male BNC. Believe me I have tried this many times and in different materials.

No I don't believe you. Use a proper tool, tighten the nut properly. Forces on a BNC connector during normal operation are minimal. When the nut is properly tightened then it won't come loose. Just look under the hood of your car and see how many things under there are tightened with bolts.

[shapirus]

No I don't believe you. Use a proper tool, tighten the nut properly. Forces on a BNC connector during normal operation are minimal. When the nut is properly tightened then it won't come loose. Just look under the hood of your car and see how many things under there are tightened with bolts.

Have you actually ever mounted a panel BNC connector like this one?

It's pretty obvious to anyone who did.

After the nut is tightened, yes, it's not easy (but not too hard either) to turn the connector even if the hole is round.

But the problem is that they actually tend to turn as you're tightening the nut, and the purpose of the shaped mounting hole is to hold the connector in place while the nut is being tightened without having to use some pliers that are quite certain to damage it in the process. There is nothing that can be used to stop it from turning in the process otherwise.

[Doctorandus_P]

Yes I have, and you do indeed have to hold the connector so it does not rotate during tightening.
The biggest problem is to know how tight the nut must be. If you over tighten it, then it's easy to strip the thread of the very thin nut. If you have never stripped the tread of such a nut, then you probably also have never tightened such a nut. And yes, you need tools to do this.

Shall we leave it at that. This thread has been derailed far enough for this silly detail.

[xvr]

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.

As I remember from KiCAD help you should draw all extra shapes before entering "Edit pad as graphic shapes" mode. Than all these shapes will be shown in list of possible shapes. All selected shapes from list will be absorbed into pad geometry. But not all shapes supported, so take a look at help before.
 
PS. I didn't try this, just help citation.

https://forum.kicad.info/t/create-pad-from-selected-shapes-solved/32770

[shapirus]

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.

As I remember from KiCAD help you should draw all extra shapes before entering "Edit pad as graphic shapes" mode. Than all these shapes will be shown in list of possible shapes. All selected shapes from list will be absorbed into pad geometry. But not all shapes supported, so take a look at help before.
 
PS. I didn't try this, just help citation.

https://forum.kicad.info/t/create-pad-from-selected-shapes-solved/32770

Yeah I've seen that thread. It's mostly irrelevant, because it was in the context of an old version of kicad (that tab in the pad properties window is long gone). The way to do it now is to use the "Edit pad as graphic shapes" context menu entry, which is not available if anything but a single pad is selected. Once you select one pad and enter that mode, you can add shapes, but only the ones drawn on the F.Cu layer are joined with the pad, and only as long as they touch the initial copper of the pad. I can understand that it's only possible to add copper to a pad, but why not bottom copper? That's weird, as a THT pad has copper on both sides, and so copper on both sides must be treated equally. Maybe I'm missing something there again.

[xvr]

IMHO you can create 2 smd pads on both layers and assign the same pad number to them. You can also add a series of through hole pads (with the same number) to join them together. KiCAD will join them in one pad effectively. I agree that it weird, but it should work at least.

[PartialDischarge]

Yes, I  think I'm going to leave it like this. That kicad thread wasn't helpful and the "Edit pad as graphic shapes" works for the external contour.

[JMK]

I'm a bit late to the party and I expect the OP has left the building; but, for future readers, here is an easy way, with Kicad, to create the required footprint.



1/ Create the hole using the Graphic Line and Arc tools on the Edge Cuts layer. (Grid .05mm, Polar Co-ords. & change dimensions of Data sheet to radii)
2/ Use Circle tool to create circle 5.15mm Rad. then edit properties to 2.4mm wide.
3/ Fill in space at bottom with Polygon tool.
4/ Place small SMT pad somewhere in filled area.
5/ Edit Pad as Graphic Shape.
6/ Add Silk, Fab, Courtyard Layers.

Note: LH symbol has different colored steps to aid description.

Finished footprint in centre. ( to change side of board use Properties and select required copper layer).
If both sides of board require the same footprint, Duplicate and change copper layer of one pad.

Estimated time for creation: 5 min.(including arithmetic ).
It took far longer to write this up than to create the pad.

I hope this helps someone in the future.

PS forgive the size of the attachment: I've only just started with "L" plates

[shapirus]

I'm a bit late to the party and I expect the OP has left the building; but, for future readers, here is an easy way, with Kicad, to create the required footprint.

Mind sharing your resulting footprint?

BTW, ideally, the edge cuts layer outline, for predictable results, has to account for the non-zero diameter of the real milling bit (see https://www.eevblog.com/forum/kicad/how-can-i-design-this-tht-footprint/msg5490496/#msg5490496).

Real bits (being say 2mm in diameter) cannot create inner corners, so it's necessary to add those "ears" where the arc meets the straight line.

[JMK]

Ok, so here is the modified internal edge cut with a reverse 1mm rad curve in place. Above it is a duplicate and mirrored arc to place at the other end of the straight cut. The rest of the drawing description is  unaltered.