Finished hole sizes after plating: how does the calculation work?

I would like to know how you cope with the finished hole sizes after plating. Let me give a very concrete example:

I have a board I would like to send to a board house. The board contains a 16-port RJ45 connector from Tyco (see datasheet). In the specs of this connector, it’s mentioned the diameter of the pins is 0.89mm or 0.035".

I don’t think I can use that value in the drill file, otherwise I’m running the risk of having holes that are too small. Or am I wrong? Is the board house itself adding extra margin to the drill holes, since they know better how much the hole “shrinks” after plating?

If not, and you’re working with different board houses, each having their own “plating thickness”, I can’t imagine one is changing all footprints each and every time. How can this be solved within KiCAD? Is there somewhere an option where you can add a fixed delta (being the plating thickness of “a” board house) to the footprint holes?

Hope you can share some experience/give advice regarding this subject.

1 Like

Try see here

[quote=“GeertVc, post:1, topic:143”]
each having their own “plating thickness”
[/quote] If that get be a problem then is you hools to small :smile:

Typically, if you’re worrying about the plating thickness, then your hole is too small. A larger-than-needed hole is rarely an issue, but a smaller-than-needed one ruins your board. If you’ve already half assembled a board before finding a hole size issue, then you’ve also potentially ruined some parts. A better approach is to simply make the hole larger than necessary, and shrink it down on later revisions as needed.

You should be fine just by following the datasheet’s suggested part layout. They take into account all the part tolerances, and add in typical fab tolerances for something that should be pretty robust. Just double check to make sure that the fab’s drill size chart supports it, and then you’ll be fine.

The precise answer for coping with the plating is that it’s fab specific. Some fabs assume that the size you specify is the “finished hole size” (eg, after plating), and some assume it’s the “unfinished hole size” which will be plated afterward.
AP Looks like an example of a fab that expects you to specify unfinished hole sizes. So, if you specify a 20 mil drill, then it gets fabbed as 20 mil, then plated, and the board has a 17 mil hole.
OSH Park is an example of a fab that expects finished hole sizes. Specifying a 20 mil hole means we select an 23 mil drill, plate it, and give you a 20 mil hole.


The last paragraph in your answer explains a lot, if not all. But then it also shows that, depending on the board house you choose, you have to take into account what they expect: finished or unfinished hole sizes.

This also means that, when you create footprints, you have to take into account the “worst case scenario”. However, while designing the footprints, you might not have any clue yet to which board house you will send your board. Hence, again the “risk” of choosing the wrong drill diameter while creating the footprint(s) for a new component…

And that is what puzzles me a bit: what’s the best approach here. Again, until now, I have no experience with board houses, I will step into the “realm of board houses” for the first time and I don’t want to shoot myself in the foot with those kind of things…

As mentioned, if you’re using a “recommended footprint” (which is a good idea), then you should be OK going with their suggested hole sizes. Those usually take into account general fab variances, so you don’t need to worry about them.

If you’re calculating the hole sized based on the pin, then I would simply add an extra 3-5 mil as a fab tolerance. That will cover most fab-specific issues, as well as rounding for their drill selection. So, an initial calculation (using a header pin as an example) would look like this:
(35 mil nominal pin size + 2 mil pin size tolerance + 2 mil clearance for fit + 5 mil fab tolerance). That gives you 44 mil, which is pretty reasonable, if not a bit generous. But, it gives you total fab immunity. Even if the fab punched this with a 40 mil drill and then plated it, the board would still work, which is what we want.

For a connector, using huge holes to cover all situations might not work out. In this example you have a right-angle connector that probably needs to fit through a hole in a panel. Your connector has huge spring-pins for alignment (0.128 holes). These pins will help align the connector as the hole size varies. I can’t tell from my quick look at the drawing if these pins are intended to be soldered or not. Sometimes the pins are quite springy intended for soldering. These would help align the connector even though there is a lot of variation in the hole size. In other cases the pins are plastic. If the pins are plastic, use an unplated hole. Then these pins will provide a more precise mounting.

In general, boards designs are not totally fab-shop-independent. Get to learn the format of the drill file so that you can edit it by hand (or with a script) as needed.

Mechanical engineers spend a lot of time worrying about manufacturing tolerances and board-shop capabilities for things like plated hole sizes of connectors. One approach is to get a sample part and try drilling different unplated hole sizes on a blank board until you get what you want. That would be difficult in this case because there are so many pins. You could instead make a test board to try a few different footprints.

Mechanical engineering of this sort is hard work and it can’t always be reduced to one number that can be used in every fab shop in the world.

As my old boss used to say about our early prototypes, “every resistor a pot and every hole a slot.”

Hi @GeertVc, so sorry for bumping such an old post, but I’ve been searching for Kicad footprints and models for this exact part and before I spend time making them from scratch was wondering if you still had yours?


I personally prefer to adopt a design style that is constant over time. I do not want to make my design PCB manufacturer specific, as you never knows where the job may end up, although I use the same PCB shops.

Drill size is no different and I go with the part manufacturer specification assuming it is the finished hole size. Most good PCB fab have an option to tick when placing the PCB order for hole size plated or not, so we are covered there. For those shops that do not have this option, then I either edit my drill file (and rename it) to reflect the proper drill size, or I drop a note in the order to increase drill size so the finished hole is the proper size.

Sure, I still have the footprints. The only thing I didn’t make, was the 3D parts, since that’s too hard for me to do (I’m not a 3D specialist…).

In the mean time, I’ve used OSHPark to create boards for me with this footprint and all went smooth. I’ve taken 0.9mm drill holes (which is the FINISHED hole size in case of OSHPark, brilliant!) to make sure I could rather smoothly fit all 128 pins at once on the PCB.

I’ve attached both the .lib as well as the .mod file. Enjoy!

GVC_RJ45_15.mod (12.8 KB)
GVC_RJ45_16.lib (13.1 KB)

You’ve saved a busy father of two several valuable hours! Thank you very much!

@Michel: for the moment I’m using the brilliant PCB house OSHPark and they take care of the extra drill space needed. If you specify a drill hole, you’re sure the finished hole is what you specified. I can for sure live with that for now.

@Darkhand: Welcome and enjoy your gained time with your youngsters!!! :smile:

[quote=“Michel, post:9, topic:143”]
I personally prefer to adopt a design style that is constant over time. I do not want to make my design PCB manufacturer specific, as you never knows where the job may end up, although I use the same PCB shops.

Drill size is no different and I go with the part manufacturer specification assuming it is the finished hole size . . .
[/quote] These days (2015), it seems to be almost universal practice for board designers, and board fabricators, to speak in terms of the FINISHED hole size (i.e., after plating, cleaning, etc - ready to be put in a box and shipped). At least that’s how it has worked with the half dozen or more fabricators I’ve worked with over the last dozen years or so. As a practical matter, that’s the most reasonable way to do it: the board designer has no insight, and even less control, over the manufacturer’s processes. The only common interface where they can interact is the finished hole size. If the board designer orders a hole of, say, 0.035" diameter, then the fabricator is obligated to deliver a hole of 0.035" diameter.

In case there’s any doubt . . . every PCB fab drawing I recall seeing for the last 20 years or so, both drawings I created and those created by others, included a note to the effect that “Hole sizes are specified after any required plating, finishing, etc.”. (Yeah, I know, not everybody bothers to read the drawing Notes, but that’s a different topic.)

So, as a first cut, if the component manufacturer suggests a 0.035" hole, then you put a 0.035" hole in your footprint. But there are two additional factors to consider. The first is plain old tolerances. Despite his best efforts, a fabricator who intends to create a 0.035" hole may actually produce 0.034" diameter. Or 0.037". Some vendors publish guaranteed hole-size tolerances on their web pages, while others need their arms severely twisted before they’ll reveal the information. Component manufacturers make allowances for practical fabrication tolerances when they suggest a hole size. If you work with a micrometer in hand, calling out hole sizes based on measurements from sample components, and expect line-on-line fits between components and holes, you’re going to be disappointed.

The second factor is drill availability. ESPECIALLY for prototype and low-rate (up to a few hundred boards) orders, the board fabricator is going to map your specified hole sizes into the tooling he typically uses. For low-volume orders, unless you throw a tantrum and pay some hefty surcharges, your boards will be fabricated with his “standard tool rack” - typically a couple dozen drills producing the most commonly requested hole sizes. You can usually find these sizes listed on the fabricator’s web site. (And no two fabricators have exactly the same list.) If you call out a hole size that matches the fabricator’s tooling, everything is fine - he’ll deliver what you asked for. More commonly, at some point in your design the hole size will NOT match his drills. E.g., you asked for 0.035" but his standard sizes are 0.033" and 0.036". Some fabricators will round up to the next larger size (0.036" in this example); others may round down to the next smaller size (0.033"); and others will select the nearest size (0.036" again for this case). In most cases the fabricator’s mapping of hole sizes produces usable results but in a few critical cases (or if you use automated insertion machines) it’s important to know how the “non-standard” hole sizes will be treated.

(I once worked with a board fabricator who insisted that the hole sizes specified on my drawing had to match the drill sizes in his standard rack before he would make the board. That put the responsibility entirely on me to specify suitable hole sizes.)


Thanks! :smile:

(I realize I’m veering way off topic here, mods feel free to split this to another thread)

I contacted the manufacturer (TE Connectivity) and it turns out they have a modeling department that will go and create 3D models of their parts for customers by request, free of charge!

It took about a week for them to create but I received it today, and it should go up on the official product page shortly. My only issue now is properly importing it into kicad!

I used FreeCAD to export the STEP file to WRL, but the scale and offset was way off. I manually tweaked it by eye, but what’s the proper way to get this file scaled to a size and offset that kicad expects, without having to enter crazy offsets?

Below is a screenshot of the part on a board I’m working on:

Impressive… Am I interested? Of course, I am… As I told you, I’m not a 3D expert and hence, I only created the drill holes for the PCB I worked on.
Would it be possible to share that 3D model with me/us?

Wanted to make sure that the file can be distributed before I uploaded it. They confirmed that it can be, and they’ll eventually have it on the part page for everyone to download:

c-5569254-1.stp (2.4 MB)

Any chance you can provide a model that is understood by KiCAD?

Sure thing! That’s the original file from the manufacturer, this one is the same file exported from FreeCAD to .wrl format. I haven’t made any changes (other than changing the color to dark grey to match the part):

c-5569254-1.wrl (2.0 MB)

The offsets I used to get the model to display correctly are:

Shape Scale:
X: 0.395
Y: 0.395
Z: 0.395

Shape Offset (Inch):
X: 2.1
Y: -0.93
Z: 0.5

Shape Rotation:
X: -90
Y: 0
Z: 0

I just eyeballed it manually until the pins lined up on your footprint, so I wouldn’t use those settings in anything production!