Drill Hole Sizes


I have a component that doesn’t have any dimensional drawings but I used a caliper to measure the pins which are approx. 0.62mm x 1.45mm. I then tried to figure out what drill size and pad size I should use. Doing some googling, I found a post that says typical sizes are .020, .025, .029, .035, .040, .046, .052, .061, .067, .079, .093, .110, .125. Translating this to mm is as follows

0.020" -> 0.508mm
0.025" -> 0.635mm
0.029" -> 0.737mm
0.035" -> 0.889mm
0.040" -> 1.02mm
0.046" -> 1.17mm
0.052" -> 1.32mm
0.061" -> 1.55mm
0.067" -> 1.70mm
0.079" -> 2.01mm
0.093" -> 2.36mm
0.110" -> 2.79mm
0.125" -> 3.18mm

Assuming there is some tolerance of 3 mil = 0.076mm my component would be max 0.62mm + 0.0762" = 0. 72mm by 1.45mm + 0.0762" = 1.53mm. So looking at the table above, I want to chose a drill hole that is just barely larger than that, i.e. 0.737mm x 1.55mm. So my questions are:

  • Does the 0.737mm x 1.55mm drill size make sense for a pin that I measured at 0.62mm x 1.45mm (note that I will have the PCB manufactured but will solder components myself).
  • How much should I add for the pad size? Is it a fixed amount or a percentage of the drill hole? In either case, how much?

Thanks in advance.


Every PCB fabricator has a list like this, giving the hole sizes they are capable of supplying for routine jobs. You may hear it called the “standard tool rack”. In nearly all cases there are no additional charges if ALL of the holes on your board are a size from the standard tool rack. (It wasn’t always that way. Once upon a time, you were charged so-much per drill, for each hole size called out on your board.)

There are four things to remember about the standard tool rack:

  1. Those hole sizes are the size AFTER plating and finishing. If a vendor wants you to specify the drill size - before he plates the sidewalls of the hole - get another vendor. He is essentially telling you that he does not have his manufacturing processes under control.

  2. Like any physical part, those sizes have a tolerance. Probably a few mils, but it varies from one fabricator to another. In fact, there are usually TWO tolerances - one for the hole diameter, and another for the location of the hole center. Don’t attempt to design your board for a line-on-line fit to any part or component.

  3. No two board vendors can agree on which sizes belong in the standard tool rack.

  4. Find out what your board fabricator does when you call out a hole size that doesn’t exactly match any standard size. Will he make the next larger hole size? Or, will he make the next smaller hole size? Or, will he put your order on “HOLD” until you send him fab files where all of the holes match one of his standard sizes?

Are you calling out an elongated (oval) slot, not just a simple round hole? That probably requires special cooperation between you and the board fabricator. Get him on the phone and make certain that he understands what you want, and you understand what he is able to supply (and the prices).

As a general rule of thumb, hole diameters are 5 to 10 mils (0.12 to 0.25 mm) larger than the component leads that go into them. If the lead isn’t round, make sure you measure the largest diagonal of the lead.

If you will stuff and solder the board by hand, hole size isn’t nearly as critical as a board being stuffed and soldered by machine.

The board fabricator refers to the copper pad around a component hole as the “annular ring”. He will require it to be a minimum width, to ensure that the plating inside the hole is anchored to the top and bottom surfaces of the board. And to make a larger target for the drill to hit when it makes the hole. (Remember what I said about position tolerance?)

I don’t recall when I saw a PCB fabricator who required more than a 10 mil (0.25mm) annular ring, though you may find somebody who has been asleep for 20 years and requires 12 mil (0.3mm) or 15 mil (0.4mm). The annular ring width will never be less than the minimum permissible trace width, and is typically a little wider. Remember that 10 mils (0.25mm) is the thickness of a business card.

For manual soldering it is better to have a wider annular ring. (More contact area for the soldering iron tip.) I typically design pads with at least 20 mils of copper around the component holes.

You will find answers to these, and many related questions, in the “Design for Manufacturing” manual published by Seeed Studio. Download a copy at no charge from “SEEED DFM Manual” .


Error trying to save custom footprint

Dale, wow, thanks A LOT for this detailed answer. This is extremely useful information. I haven’t decided on a manufacturer yet but will check their website for drill sizes and if they don’t list it contact them so I can put in exactly what they offer. And yes, a few of the vias are oval because that is how the pins are. I was a bit concerned about that. I will just go with a circular one and hope when soldering it will fill it nicely.

I didn’t go through the entire document yet but it already opens questions that I never thought of before. For instance on page 14 Figure 12 they say that if a trace is wider than a pad then the two should connect with a trace that is even narrower than the pad. That’s kind of a concern for me because I have MOSFETs each handling about 6A. I currently have it like this:

So the center pin (Drain) has a track that is wider than the pad. Is it ok if I reduce it to exactly the pad width and then I can connect it directly? I also assume they are only concerned about the pad and not the drill hole. Note that on the backside I have the same trace (I am not showing the back layer in this image) so I am doubling it.

Then just below (Figure 13), why shouldn’t you connect them directly? Because copper would pool up there?

Then again just below (Figure 14) I assume the hole is the white part. Why is the pad not centered around the hole? And then what is the light yellow part? Additional padding? How do you do that in KiCad?


These are probably anchoring pins for connectors or switches. Elongated, or oval, holes are a long-standing problem with inexpensive, quick-turn boards. Many fabricators do not support them at all. Others impose a surcharge. A few will permit you to approximate them with overlapping drill holes, even though that violates their minimum hole-to-hole spacing. I recall a Forum thread from a month or two ago that discussed dealing with one fabricator’s offering.

I have avoided elongated holes on prototype boards. Like you, I call out a round hole with a diameter right at, or very slightly over, the largest tab dimension to be inserted. With manual soldering I have usually managed to pour enough solder in to fill the hole, or at least firmly anchor the pin. The key is to have enough WATTAGE in the soldering tools - I often use TWO of the Hakko FX888’s (50W each, I think) to solder switch tabs and connector frames. Jacking up the tip temperature to a zillion degrees isn’t the same thing - doing that makes it more likely that I’ll leave a trail of scorched or delaminated spots on the board around the tab.

That trace-to-pad connection geometry may have something to do with the PCB fabrication process (concerns for over- or under-etching in confined areas), but I’ll wager it’s related to getting a good solder joint between the component and the pad. The wide trace pulls heat away from the pad, causing it to heat less uniformly than the other IC pads in Figure 12 and a potentially less secure solder joint. A short length of narrow trace keeps more heat in the pad. I wouldn’t expect that kind of problem in a modern reflow oven that goes to great lengths to heat everything very uniformly, but it’s my best guess to justify Seeed’s requirement. Or perhaps they’re thinking about manual soldering and re-work, where soldering SMT devices is much more troublesome.

For the TO-220 MOSFET on your hand-soldered board, ease of soldering is almost certainly the main concern. I would neck-down the trace to the Drain for 0.1" (2.5mm) or so from the pad, and add thermal relief spokes to the Source pad.

The question, “How wide should a trace be?” has no easy answer. To start with, you must define what a trace “failure” is. Is it de-lamination of the trace from the substrate? The voltage drop across a length of trace? A certain temperature rise in the trace? System power dissipated by the traces? Vaporization of the trace? You can start to appreciate the complexity of the question by opening the “Calculator Tools” in KiCAD’s main shell and going to the “Track Width” tab.

Setting aside those (very real) details, many design guidelines will suggest that 1 amp of current can be handled by a trace of 1-ounce copper that is 10 - 12 mils wide, on boards operating in common, benign, environments. That suggests a 60 - 80 mil trace, or three 25-mil thermal spokes should be adequate.

Here again, I don’t know if SEEED is concerned with board fabrication or assembly solderability. I have never hesitated to make direct connections between pads, though I place them at the far edge of the pad, away from the IC body.

I don’t know what SEEED is trying to show in Figure 14. It may be addressing situations (like the anchor pins for connectors or switches) where mechanical strength is a significant concern, as well as electrical connectivity. If they’re telling us that holes may not be exactly positioned (which is true, and unavoidable) then I’d deal with it by making the pad a little larger, or possibly elongating the pad in the direction of the trace attachment point.

With KiCAD’s through-hole pads you can specify a pad shape that is shifted from the hole center using the “Offset” parameters.

And here is a power “barrel jack” where I elongated and offset the pads with the intention of achieving stronger, manually-soldered joints.



This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.