Avoiding additional costs when designing PCBs for components for slotted holes - Page 1
Forum section: electronics / beginners

author: jameswilddev
author_rank: Contributor
timestamp: February 16, 2021, 08:00:16 pm
content: I have a lot of these PCB mount DC jacks and I'd like to get a PCB made using one:I've used the KiCAD DC jack footprint and it's a perfect match (this is a 3D printed dummy to make sure everything fits):However, a local prototyping service I'd like to use has complexity/price tiers, and adding a slotted drill hole nearly triples the price per board as my board is otherwise very simple.Given that I have a 3D printed case which mechanically secures the connector and PCB anyway:Could I get away with just having a really big round drill hole to avoid this fee, or is this a very a bad idea? Worst comes to worst I could fold the flat pins down to the PCB to get a better mechanical fit as they're 2.5mm clear?

author: Benta
author_rank: Super Contributor
timestamp: February 16, 2021, 08:59:49 pm
content: Place 3 or 4 holes in a row so they overlap a bit. The CNC drill normally doesn't care.The big hole idea is bad, as it needs manual rework for bending the leads.

author: David Hess
author_rank: Super Contributor
timestamp: February 16, 2021, 09:55:00 pm
content: Quote from: jameswilddev on February 16, 2021, 08:00:16 pmThat is what I do and it has never been a problem.

author: ataradov
author_rank: Super Contributor
timestamp: February 16, 2021, 10:56:03 pm
content: Quote from: Benta on February 16, 2021, 08:59:49 pmI'm sure their CAM won't let you do this. Carbide drill bits break if they try to drill overlapping holes.Round holes are fine, but they consume a ton of solder.All Eagle footprints use giant holes, and they are fine. Look at the original Arduino board. It had big holes.

author: Benta
author_rank: Super Contributor
timestamp: February 16, 2021, 11:07:10 pm
content: Quote from: ataradov on February 16, 2021, 10:56:03 pmDepends on the manufacturer. Some do, some don't.

author: tszaboo
author_rank: Super Contributor
timestamp: February 16, 2021, 11:11:30 pm
content: Quote from: ataradov on February 16, 2021, 10:56:03 pmI was also under this impression, but a lot of mechanical keyboards do this, to allow different keyboard layouts on the same pcb. Some of them is like swiss cheeses with so many overlapping holes.

author: ataradov
author_rank: Super Contributor
timestamp: February 16, 2021, 11:15:41 pm
content: It probably depends on the diameter too.For a slot you will want 1mm or bigger, so it may be fine. But they will still may want to charge extra for that.

author: mvs
author_rank: Frequent Contributor
timestamp: February 16, 2021, 11:48:23 pm
content: Quote from: jameswilddev on February 16, 2021, 08:00:16 pmIs it a general rule for slots or is just because of small slot width in this case?Big holes are usually milled anyway, so it should not make a large difference for PCB fab.

author: jameswilddev
author_rank: Contributor
timestamp: February 17, 2021, 12:10:13 pm
content: In this case a general rule for slots. I've uploaded files with both slots and massive drill holes and it only triggered the rule for the former.An example of an existing PCB with massive drill holes (thanks for the idea of looking up Arduino):

author: Renate
author_rank: Super Contributor
timestamp: February 17, 2021, 12:56:10 pm
content: Ew, ugly big holes. You need a roll of solder just to fill them.The standard biphase encoder knobs have two big mounting tabs.I've had nice plated 1 mm slots milled in a big oval pad.Osh Park did that from an Eagle-generated Gerber .gko file.It turned out fine.In the Eagle definition for the encoder package it's just:Code:<wire x1="-0.889" y1="6.35" x2="0.889" y2="6.35" width="1.0" layer="46"/><wire x1="-0.889" y1="-6.35" x2="0.889" y2="-6.35" width="1.0" layer="46"/>Layer 46 is "milling".The interesting thing is that there are two different phases for drilling/milling.The first phase is on the unetched board before plating.The second phase is on the finished board for unplated holes.Or am I wrong about all this?Since the Excellon drill file .xln and the .gko only have one instance they must somehow sort them into "before" & "after"?Osh Park says that they'll handle plated slots in a .gko as a legacy feature, but they'd prefer them in the .xln file.I'd have to manually insert them in the .xln file.I wonder how they determine a mill vs. a drill in the .xln file?Do they scan through and see which operations have movement?

author: jpanhalt
author_rank: Super Contributor
timestamp: February 17, 2021, 01:17:07 pm
content: Oshpark has a nice discussion on plated through slots (PTS) -- at least it did last year. It lists some manufacturers that have no problem with it and specifically points out that Eagle prior to 8.0 is an exception.In sum:1) With Eagle versions prior to 8.0, Oshpark has a CAM modification. That worked fine for me and was no additional cost to Oshpark's usual charge.2) Autodesk Eagle CAM may support them. An Autodesk rep. commented in the Oshpark discussion, but I didn't pay much attention to it.3) JLCPCB said they could do it, but never responded whether a trial approach I submitted would accomplish it. There are a few ways to do it. One of which is to design the slot and add a PTH pad. Another is to just be sure you have copper connected to the appropriate net on both sides of a slot.4) Check with the manufacturer you plan to use.Just FYI, I was adding an Omega TC and other sockets to the board. I am quite happy that I paid Oshpark to make the PTS rather than use big holes.

author: wraper
author_rank: Unknown
timestamp: February 17, 2021, 01:23:39 pm
content: QuoteThen don't bring business to them. Most of Chinese services make plated slots at no additional cost. And they are way cheaper to begin with.

author: tszaboo
author_rank: Super Contributor
timestamp: February 17, 2021, 01:40:15 pm
content: To answer the original question, check if they charge extra for 0.5mm slotted holes, or 1mm. Maybe just charge extra because your hole was too narrow.Or you might try it as NPTH, instead of PTH, and just solder it from two sides. Unless you want to sell it, it should be OK.

author: Renate
author_rank: Super Contributor
timestamp: February 17, 2021, 01:46:25 pm
content: Oh, one thing that I noticed about Eagle 7.7.0 (which may not be true of your version).If you specify a pad with x, y, diameter, shape but no drill it will default to a drill size of 0.0When you CAM it you will see that these "zero size" drill holes are in the .xln file.I use an editor script to strip the "zero size" holes out, remove the "zero size" tool and renumber the tools.OTOH, everybody seems to ignore "zero size" holes.I think Osh Park has a minimum of 1 mm for milling.

author: jpanhalt
author_rank: Super Contributor
timestamp: February 17, 2021, 06:54:22 pm
content: Quote from: Renate on February 17, 2021, 01:46:25 pmThe board I submitted last Spring had 0.5 mm wide slots for mounting a USB port. They came back perfect and no questions were asked.