How can I design this THT footprint? - Page 1
Forum section: electronics / general

author: PartialDischarge
author_rank: Super Contributor
timestamp: May 08, 2024, 11:39:52 am
content: 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.

author: shapirus
author_rank: Super Contributor
timestamp: May 08, 2024, 01:39:38 pm
content: 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.

author: PartialDischarge
author_rank: Super Contributor
timestamp: May 08, 2024, 02:05:28 pm
content: Quote from: shapirus on May 08, 2024, 01:39:38 pmExactly, 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 rotationQuoteI 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

author: golden_labels
author_rank: Super Contributor
timestamp: May 08, 2024, 04:30:37 pm
content: 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?

author: PartialDischarge
author_rank: Super Contributor
timestamp: May 08, 2024, 04:59:58 pm
content: Quote from: golden_labels on May 08, 2024, 04:30:37 pmThere 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.QuoteOnly the ground will connect directly to the PCB, the other central pin of the BNC needs a cable of course.

author: Doctorandus_P
author_rank: Super Contributor
timestamp: May 08, 2024, 05:59:06 pm
content: 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 ofEdge Platingand 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.

author: shapirus
author_rank: Super Contributor
timestamp: May 08, 2024, 06:05:11 pm
content: Quote from: PartialDischarge on May 08, 2024, 04:59:58 pmAh, now, that's the right way of phrasing the question :).Nope, it looks like this isyet anotherreal 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/25859/11as usual, hard to understand if it's still applicable because of all the changes in the UI.

author: shapirus
author_rank: Super Contributor
timestamp: May 08, 2024, 06:12:55 pm
content: Quote from: Doctorandus_P on May 08, 2024, 05:59:06 pmDon't all slots and holes get platedby defaultunless 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?

author: shapirus
author_rank: Super Contributor
timestamp: May 08, 2024, 06:16:06 pm
content: Quote from: Doctorandus_P on May 08, 2024, 05:59:06 pmBesides, 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.

author: gamalot
author_rank: Super Contributor
timestamp: May 08, 2024, 06:27:04 pm
content: Like this.

author: shapirus
author_rank: Super Contributor
timestamp: May 08, 2024, 06:32:04 pm
content: Quote from: gamalot on May 08, 2024, 06:27:04 pmThat's how it'll actually be milled. But how do we make this shape a hole in a plated THT pad in kicad?

author: PartialDischarge
author_rank: Super Contributor
timestamp: May 08, 2024, 06:34:29 pm
content: Quote from: shapirus on May 08, 2024, 06:05:11 pmExactly that's something quite similar to what I'm trying to do. I'll read that thread...

author: shapirus
author_rank: Super Contributor
timestamp: May 08, 2024, 06:37:21 pm
content: Quote from: PartialDischarge on May 08, 2024, 06:34:29 pmLet us know what you end up with. That's not an unusual task, yet quite unclear as to how to do it in kicad.

author: golden_labels
author_rank: Super Contributor
timestamp: May 08, 2024, 10:44:15 pm
content: 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 fromJLCPCB.

author: Doctorandus_P
author_rank: Super Contributor
timestamp: May 09, 2024, 01:28:48 am
content: I had a look at the Gerber X2 standard.Apparently there is a.FileFunctionforPlatedrouting. 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 MixedBut 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.FileFunctionwith 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.

author: PartialDischarge
author_rank: Super Contributor
timestamp: May 09, 2024, 04:36:16 am
content: Quote from: golden_labels on May 08, 2024, 10:44:15 pmThat 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

author: forrestc
author_rank: Unknown
timestamp: May 09, 2024, 06:16:21 am
content: Quote from: PartialDischarge on May 09, 2024, 04:36:16 amI 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.

author: PartialDischarge
author_rank: Super Contributor
timestamp: May 09, 2024, 08:46:10 am
content: 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.

author: Silenos
author_rank: Regular Contributor
timestamp: May 09, 2024, 11:49:25 am
content: 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.

author: golden_labels
author_rank: Super Contributor
timestamp: May 09, 2024, 01:31:36 pm
content: 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 designedand optimizedto 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.

author: PartialDischarge
author_rank: Super Contributor
timestamp: May 09, 2024, 01:43:30 pm
content: Quote from: golden_labels on May 09, 2024, 01:31:36 pmI 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....

author: shapirus
author_rank: Super Contributor
timestamp: May 09, 2024, 02:30:42 pm
content: Quote from: PartialDischarge on May 09, 2024, 01:43:30 pmAlso, plated oval slots seem to be pretty standard (no added cost).

author: golden_labels
author_rank: Super Contributor
timestamp: May 09, 2024, 06:39:05 pm
content: 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. /sIf 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.

author: forrestc
author_rank: Unknown
timestamp: May 09, 2024, 08:39:50 pm
content: Quote from: PartialDischarge on May 09, 2024, 01:43:30 pmI'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).

author: PartialDischarge
author_rank: Super Contributor
timestamp: May 10, 2024, 04:18:25 am
content: Quote from: forrestc on May 09, 2024, 08:39:50 pmAnd 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

author: forrestc
author_rank: Unknown
timestamp: May 10, 2024, 05:02:33 am
content: Quote from: PartialDischarge link=topic=427450.msg5492524#msg5492524I 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.

author: vk4ffab
author_rank: Frequent Contributor
timestamp: May 10, 2024, 05:54:37 am
content: Quote from: PartialDischarge on May 08, 2024, 11:39:52 amNot 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.

author: Doctorandus_P
author_rank: Super Contributor
timestamp: May 10, 2024, 06:29:49 am
content: 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.

author: PartialDischarge
author_rank: Super Contributor
timestamp: May 10, 2024, 06:36:07 am
content: Quote from: vk4ffab on May 10, 2024, 05:54:37 amYes that's what I'll end up doing for simplicity

author: PartialDischarge
author_rank: Super Contributor
timestamp: May 10, 2024, 06:38:12 am
content: Quote from: Doctorandus_P on May 10, 2024, 06:29:49 amAbsolutely 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.

author: Doctorandus_P
author_rank: Super Contributor
timestamp: May 10, 2024, 07:04:42 am
content: Quote from: PartialDischarge on May 10, 2024, 06:38:12 amNo 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.

author: shapirus
author_rank: Super Contributor
timestamp: May 10, 2024, 08:52:45 am
content: Quote from: Doctorandus_P on May 10, 2024, 07:04:42 amHave you actually ever mounted a panel BNC connector like this one?It's pretty obvious to anyone who did.Afterthe 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 placewhile the nut is being tightenedwithout 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.

author: Doctorandus_P
author_rank: Super Contributor
timestamp: May 10, 2024, 09:10:34 am
content: 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.

author: xvr
author_rank: Frequent Contributor
timestamp: May 10, 2024, 08:53:23 pm
content: Quote from: shapirus on May 08, 2024, 06:05:11 pmAs I remember from KiCAD help you should draw all extra shapesbeforeentering "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

author: shapirus
author_rank: Super Contributor
timestamp: May 11, 2024, 12:35:39 am
content: Quote from: xvr on May 10, 2024, 08:53:23 pmYeah 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.

author: xvr
author_rank: Frequent Contributor
timestamp: May 11, 2024, 06:43:45 am
content: 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.

author: PartialDischarge
author_rank: Super Contributor
timestamp: May 11, 2024, 07:52:21 am
content: 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.

author: JMK
author_rank: Contributor
timestamp: May 15, 2024, 09:33:25 am
content: 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

author: shapirus
author_rank: Super Contributor
timestamp: May 15, 2024, 10:11:57 am
content: Quote from: JMK on May 15, 2024, 09:33:25 amMind 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 (seehttps://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.

author: JMK
author_rank: Contributor
timestamp: May 15, 2024, 12:39:34 pm
content: 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.