Public footprint libs - Is there a reason for having (some) so tiny THT pads?


I’ve started using Kicad some months ago, basically to design some simple circuits for my classes. These circuits are intended to be drilled and soldered by hand by my students, most of them having little soldering knowledge.

The problem is that I find myself editing again and again the default pad size of usual THT components (DIP sockets, discrete components, etc.) to make it bigger, because the default pad size is too small to be manufactured by hand, as drilling removes most of the pad’s copper.

So I wonder why is the (majority) footprints default pad size so small. Is there any reason/ design decision that justifies it? And, if not, is feasible to submit a proposal to increase the pad size that comes into the libraries (only for certain components, of course)?


Without meaning to be mean, but have you thought about setting up a ‘personal class’ library of vetted footprints that suit your use case and only use those for projects with your students?
Did you know that there are scripts that come with KiCAD that enable you to semi-automate footprint creation which can be tweaked to your personal liking?

The majority of the public KiCAD footprints will adhere to the respective standards (be it JIS or DIN or whatever) as they are being created by scripts and if that doesn’t apply, the actual datasheet will have been followed (or should have been).
But definitive answers can only be given by the library maintainers and if they don’t see this here you might want to contact them on github via the bug tracking system on there.
Oh, and best would be to have examples handy.


You need to follow @Joan_Sparky advice about creating your own class library for THT components for hand drilling. Something like this already exists in the SMD parts with larger pads for hand soldering.

The reason for the default sizes is that the vast majority of KiCad user are getting their boards made by commercial PCB fabs and we follow the standards for pad sizes. Larger pads makes it impossible to route tracks between pads. There is no problem hand soldering THT components made with standard pads, your problem is due to hand drilling.


You are teaching students skills they will never need. No one in the industry drills or boards by hand, and hand soldering is the exception. KiCad libraries are designed for real world usage. Since you can buy 10 boards for $2, even amateurs and hobbyists don’t bother making their own boards.

If you wish to teach students practical skills, how about making their first assignment designing some footprints… after a few years you will have a comprehensive library.


Some of the prior replies seem to me to be a little more hostile than they should towards a newcomer to KiCad and the forum.

Let me sum-up with snippets:

@orestesmas What is the exact size of the footprints you are having problems with? And, what is the exact size of the holes you are drilling for through-hole parts?

ON EDIT: WELCOME to the KiCad User Forums!


I see statements of fact rather than hostility. But if your first post is unreasonable criticism of the hard work created by volunteers, rather than thanks them for their efforts, what do you expect?

It’s like going to a dinner party and telling the host you don’t like their cooking, and “next time make something I like”.


I did not read the OP that way; because these two lines were in the OP:

To me, the OP clearly did not mind editing one or two pads to the library Footprints, but wished to fix it, or at least know why it was the way it was. I don’t see any fault in the OP’s queries.


Hi Orestes,

I think the main reason is that footprints are thought to be machine soldered.
Pads are usually smaller to preven paste waste and mostly to prevent the component floating too much on the solderpaste during soldering. Some forum members will disagree with my statements

Anyway, I have found that different manufacturers want different pad sizes for the same component. So I think it also depends on the machine and the operator skills.

For manual soldering we need bigger pads. There are some footprints in the official libraries focused on manual soldering, anyway. I agree the official libraries should be focused mainly in machine soldering.


Of course you’re right: doing things by hands is not the way to go in the industry. Even in the hobbyist world with the popularisation of cheap PCB fabrication companies. But I still consider of pedagogical value going through the entire process of CAD a board, printing the layout, doing the toner transfer, etching the board, drilling and soldering. It’s an intermediate step between wiring a prototype circuit board by hand and sending te design to fabrication. It also helps demystifying circuit design. Moreover, sending the PCB to a fabrication company takes time and may not fit well into the course schedule.

But maybe I’m wrong and I’ll have to reconsider the course orientation in the future.


In several counties etching a PCB at home or in a school/college environment is getting tricky because of the chemicals used.

Some KiCad users are using CNC milling to make prototype PCBs, introducing another set of constraints to the PCB design.


You need to follow @Joan_Sparky advice about creating your own class library for THT components for hand drilling. Something like this already exists in the SMD parts with larger pads for hand soldering.

Yes, perhaps I’ll have to follow this advice in the end, but before starting such a task (which may become large), I wondered two things:

  1. Why don’t exist THT components with larger pads, but they do with SMD.

  2. If there are users with the same needs, to try to share efforts on creating a class of THT components with characteristics more suitable to hand manufacturing.

There is no problem hand soldering THT components made with standard pads, your problem is due to hand drilling.

I agree, in most cases. But sometimes you have a component requiring a specific drill diameter that, when drilled (even with machine precision) the remaining pad’s copper is so tiny…


My apologies if you interpreted my post as unfair criticism. I’m myself a long-time volunteer in the free-software world (mostly contributing translations and advocating, as I’m not a programmer), and I greatly appreciate the immense effort and value of KiCad developers and contributors.

My question was motivated by pure interest and curiosity, and to know if there are more people with similar needs as mines.


Hi, I am producing my simple PCBs at home and for me all THT-Pads are also too small.
And it is true: the library is, and should, be made according to professional manufacturing standards.

But one big advantage of KiCad is: it allows you to change any Pad later without changing the library. And with V5 you can do really weird things to Pads :wink: - should be sufficient for any purpose.

Of course this is additional work but to me it is an acceptable compromise.


Well, one of our members here wrote some time ago that ECAD is 80% library work… which is exactly the thing you’re having a ‘problem’ with now.
So if you really want to teach your students something, get them to make a footprint each or at least modify the ones they need to get them to your liking.
Even at a pace of maybe 1 footprint per 5 minutes and maybe 10 people, after 60 minutes you should wind up with 120 modified footprints for the special parts and if you take care of the script-able ones as I told you this should give you enough for years to come.


Most footprints in the official lib are script generated. SMD footprints should mostly follow IPC suggestions (The ones that are scripted at least. I have not come around to script all of them at this point in time.) These suggestions take into account current manufacturing capabilities. (The current standard is a few years old now. A new one might come out within the next few years.)

At least for two terminal SMD components (SMD resistors, capacitors) we also include versions with increased toe fillets for handsoldering. (Toe fillet increased by 0.15mm. I solder the 0603 variant regularly by hand without problem. I even used the 0402 one a few times now.) However you can adapt the respective parameter in the script and generate your own footprints if that increase is too small for your liking.

For THT resistors and similar the script is not that easily modified (There is no parameter that controls drill size/annular increase. All these values are hard-coded instead of being calculated from the lead diameter.)

The THT IC packages (DIP) have a longpad version which is intended to be used when handsoldering. Other IC packages do not come with such a footprint. (They are still hand solderable with a bit of skill.)

The scripts can be found here:


I think you need to look at your drilling procedure? Do you etch or drill first? When you say hand drill do you mean free hand or drill press? Are you using hardware store bits?


I think you need to look at your drilling procedure?

Probably. Over the years we have changed/improved our fabrication procedures mostly abandoning the UV-exposing process in favor of toner-transfer techniques. But drilling remained essentially the same.

Do you etch or drill first?

Etching first.

When you say hand drill do you mean free hand or drill press?

We have a drill press in our lab. It does a fairly good job, but it’s not a tool specifically designed for drilling PCB. A CNC drilling machine is out of budget.

Are you using hardware store bits?

Yes. Any advice on that?


You should use sharp carbide bits. Something similar to these:

You can find them all over the place, I just grabbed the top non-ad google search for “pcb drill bit”. Many of the electronics vendors like DigiKey, I think SparkFun and/or Adafruit carry them, and I’d be surprised if you couldn’t find them on E-Bay. When shopping for the best price, look for the “re-sharps”. Those are bits that have been sharpened but no longer match the tolerance of the manufacturers. They should be “close enough” for the home-gamer though.

EDIT: FYI, these types of bits are made for high-speed drills (2k-3k rpm range). Standard drill presses aren’t fast enough. But a dremmel-style rotary tool with a drill-press attachment should work a treat.
Something like this: (Again, no particular preference for either Home Depot nor the Dremmel brand. Just the results of a quick search for what I was thinking about.)


I looked into doing my own boards but the price of setup wasn’t even close to justified when you look at what commercial boards cost now. But, in my studies I did see people drilling first. More copper backing to reduce the chance of tearing thin traces.

The drill bit question was already answered. Type and speed counts. Also, look at adding some kind of lubrication. I’d think slow feed in tiny nibbles would help keep the copper in tact but that is just a guess.


I think you are correct and have the best approach. People who design circuits, as well as people who lay out PCB’s, should have a basic understanding of the fabrication process. Sort of like the people who pack parachutes - they should be required to jump once in a while.

I am probably that guy. Not always 80%, but it’s not unusual for library work to be 80% of the total effort on a project that’s totally new and unlike any other recently designed project.

I agree that learning to make footprints and symbols is an important skill for anybody who does more than a board or two per year, but I don’t think that it’ll be efficient to build a working library from a collection of classroom exercises. (Of course, I may be underestimating your students.) If you put forth the effort to make your custom library comply with KLC, please submit it to the KiCAD librarians. They may incorporate it into the KiCAD libraries, thus ensuring your immortality!

(Note on footprints for hand-drilling: Manual drilling works best when you etch away a little dimple at the center of the copper pad. This creates both a visual target and a mechanical guide for the drill bit to align with. KiCAD doesn’t have the ability to create this pad style automatically (unless it slipped into version 5 when I wasn’t looking) but it’s a feature you can incorporate into your custom footprint library. More discussion at Enable drill marks for Gerber files .)

Ordinary twist drills from the hardware store are not good choices for PCB work. The standard tip geometry does not make clean entry or exit holes, and the fiberglass PCB material dulls the drills quickly. The carbide bits mentioned by @SembazuruCDE are a better choice. You probably know that half a dozen sizes will cover about 99% of the holes you need, and you will design your custom footprints around those sizes. Their major disadvantage is that they break easily, so keep plenty of spares on hand.

To minimize broken drill bits you should also pay attention to runout (slop) and eccentricity (wobble) of the chuck holding the bit. I don’t know a particular make and model to suggest, but I DO know that Dremel-style hobby tools come in several models and grades, and bearing quality is often the major difference.