New to kiCad, does a footprint exist for SPST NO THT Switch


Note that this is my first project with KiCad and I have the schematic finished and am assigning the footprints to the components.

When it came to selecting a foot print for SWITCH TACTILE SPST-NO 0.05A 12V

I could not find a foot print that matched the switch. The switch is 6mm by 3.5mm with it legs making it a bit bigger.

In the Assign Footprints, I went through all of the switches and could not find a footprint that matched the switch that I have.

Question. Does this mean there is no footprint for my switch?

I really probably should not do this…

TL1107W.kicad_mod (876 Bytes)
TL1107W_2.kicad_mod (1.3 KB)

Took me 10 minutes total. It is NOT KiCad library rules compliant.

Pad dimensions are in mm, and the drill is imperial #55.
The annular ring may appear a little small, but it does comply with OshPark requirements for fabrication.

Fab layer contains the outline of the package.

Silk layer has lines for alignment.

TL1107W_2.kicad_mod (1.3 KB)
Changes made:
Increased the annular ring size a moderate amount.
Changed the resulting pad size to a 2 decimal mm value.
Added F.Fab layer lines to resemble the approximate pin locations.

1 Like

thanks for the quick reply. I copied the file to my KiCad libraries directory under Buttons. Then I was able to select the button. It does look correct.

At this point I am laying out the board. When this is complete and I am able to print the PCB layout to scale, I can check the size against the switch.

again Thank you very much.



For amusements sake I did a search for pushbutton switches in Octopart which returned slightly less than 15,000 possible hits. Obviously many of these will be minor certification differences /duplicates / unavailable / no longer in production / EOL but the point is that there are an unbelievable variety of them. And that’s just switches.

Many beginners ask ‘Why is there no footprint for my xyz component? I can’t believe that this software doesn’t come with that pre-installed’. That is then followed by a lengthy trawl around the shady parts of the internet trying to find a matching footprint. Probably an hour or so of head scratching later you give up or place something you are a bit dubious about which you worry about until your board arrives (and possibly beyond when you find it doesn’t fit!). The lack of footprints is not unique to KiCad - even if you pay big bucks for Altium etc - you are not guaranteed to get a footprint for every component that you can order.

Sooner or later (and probably sooner), you will find that you will need to make some of your own footprints because not everything is or could be provided in the KiCad libraries. As @Sprig proved - designing your own need not take a long time, you can design the footprint to fit your manufacturing process and whatever standards/modifications you favour.

Have a look at some of the tutorials and try a few simple designs - a switch like this is a really good starter project. Look at the data sheet and follow the suggested layout. You will end up being more productive and you can be sure that the footprint meets the manufacturer guidance - and not have to trust that someone else has done it correctly. (Although the one provided above looks fine and you must owe Sprig a :beer:!).


@John_Pateman To be clear, it actually took me a little longer than I expected because it was not initialy obvious to me which section to use in the datasheet.


The F.SilkS layer informatioin provided is recommended by a local manufacture. There Quality Control system takes images of the board after manufacture and the lines in the footprint provide for their system to ensure that the part is in proper alignment. Note: they also prefer some silkscreen under the part, to make it easer to detect an unpopulated part.

The F.Fab layer information provided is because I want that information there. I use it as a “sanity check” in reference to the pads of the footprint. Here is an example:

Notice how the “blue rectangle” matches a 3D model Step file:

Using a #55 drill hole size with an Excellon drill file in inches/2:4 format should eliminate any chance of rounding error confusion.

While my footprint may not be KiCad library compliant, KiCad is not going to manufacture nor populate the boards that I produce. A wise member on this forum once told me to think of datasheet land pattern data more like a serving suggestion. That really made sence to me once I realized that different manufactures of the same package/housing part, can have differing land pattern recomendations.

Hope this information helps someone else learn how to make pcbs with KiCad! And, note, pin one of both footprints is on the left on purpose…


Some time ago I made:


I wonder if an updated version might be useful as a pinned topic. Maybe start splitting up some of the stuff that might go into the FAQ into the specific sections? Mini index pinned pointing to stuff in the FAQ? Obviously just thinking out loud here.


  1. To be honest, if if were my board, I’d probably use the smaller pad size. I was double checking the footprints for errors when I noticed that the datasheet did have an indication that the pin width was 1.00mm. The second model, the “E” version gives the specification and the other drawings and images appear to be the same scale.
    With a 1.3mm drill hole, the 1 x 0.3mm(pin thickness) is going to require quite a bit of solder just to fill the drilled hole. I only increased the pad size because I don’t know the OP’s ability to hand solder. The larger pad size should make it a little bit easier to solder.

  2. This was an oversight on my part. The whole reason for looking for errors was because when I first created it I was making an apptempt to see how fast and accurate I could create the footprint. I have the minimum anular ring size for OSHPark (not a sponsor) memorized in mils. I simply forgot to make the conversion to mm.

  3. This was not a mistake or oversight. I did not want to guess at the pin dimensions. Having since discovered a dimension on the datasheet I am now comfortable including pin drawings on this layer. Note however, that I use these simply as a “sanity check”; in other words, “close counts”.

I hope some found some insite for me sharing the why of making these changes.

1 Like

And if it was my board:

I’d order the part, and while waiting for its arrival, I’d use that time constructively to learn how to make a footprint in Kicad.

Upon the parts arrival I would then measure that part and use my newfound skills to make a footprint.

The footprint would have the largest pads I could get away with, together with large tracks joining the pads, and I would use the largest amount of solder I found aesthetically pleasing to join the switch to the pads. All these measures are to ensure reliability and robustness because a human is going to push that switch an untold number of times with an unknown amount of force :slightly_smiling_face:


These TACT switches can have leads that are hard to solder. You want big pads so that they don’t lift off while soldering

1 Like

With those THT parts, in plated through holes, you already have a pretty sturdy connection.

(Picture taken from Digikey link above)

The bent snap-in pins also promote good fitting on the PCB, with the (small plastic standoffs) on the switch making contact with the PCB.

Also, from the Datasheet:

The 3.5mm long pins give enough stickout to heat them with a soldering iron (or solder wave) A bit bigger pads then usual for stuff pushed by monkeys generally is a good idea though.

1 Like

The above critisizms are fine with me. There can be any number of reasons for making design choices. One of the reasons for leaving the original file was so that discussion on this could continue.

A significant reason for me prefering to use the smaller pads is because it is a PTH part. These cause two issues.

  1. They take up board Real Estate on both sides of the board.

  2. They create a Trace Wall on both layers.

What is a Trace Wall?

Note: Image is for simple demonstration purposes only.

For a device with only 2 pins, as shown, it typicaly is not that big of an issue. The problems start when there are more pins along with wider trace widths that required due to current draw.

Choose whatever works best for the design at hand. Be mindful though, that another design may make other tradoffs.

1 Like

Switches and connectors are probably the last categories of components where thru-hole versions are still readily available, and often preferred, over SMT versions. In spite of manufacturers’ claims, experience seems to confirm that leads or pins, anchored in plated-through holes, are significantly more rugged than flat leads sitting atop an SMT pad.

I recently had to revise a board to accept an SMT version of a switch, because it was available while the thru-hole version - that we had used for several years - suddenly had availability problems. (Can you believe lead-times over a YEAR??)

In my heart and in my mind I was opposed to the change, but when they grab you by the gonads, your heart and mind will quickly follow. I drafted a new footprint, that would accept either the SMT or the thru-hole version of the part. (The astute observer will recognize that this is another reason why you should learn to create footprints.)

That’s when I noticed that the SMT version of the switch had a significant difference from the thru-hole version. The sheet-metal framework that enclosed the switch and held it all together featured two thru-hole tabs for mounting and positioning. The part was “SMT” in name only - to achieve the best reliability, you still have to do a thru-hole soldering step on those tabs! In fact, because the switch leads splayed out from the body to connect on SMT pads (“gull-wing” style), the top-side footprint for the SMT version used more acreage than the thru-hole version. And, even though the thru-hole part used space on both sides of the board, those mounting tabs used almost as much space on the back side of the SMT footprint. In short, I don’t see that the “modern” SMT version is a real improvement over the “old-fashioned” thru-hole version.



Thanks for that question! As others mentioned, it has been asked before, but it is still a common, and relevant, question for people new to PCB-Layout software in general.

When I first started paying attention to PCB software about a quarter century ago, I was impressed by the publishers who claimed, “Our software include a jillion footprints.”. Of course, the next guy said, “Well, mine has over a zillion footprints.”.

Now (perhaps in no small part because I’m a bona-fide, genuine, certified geezer) I know that’s all marketing hype. The REAL way to evaluate a layout program is by how easily you can draft, and integrate, your own symbols and footprints into the software. Every organization I’ve worked with has created and maintained their own custom library of symbols and footprints. After scanning through this thread, it should be apparent that there are numerous justifications for doing this, and no publisher-supplied library - regardless of size - will ever be a one-size-fits-all solution.



Like my grandkid riding a bicycle without touching the handlebars, I think you just wanna show off!

Once you “get” something, it’s easy. You forget about the time, effort, and mental strain of figuring it out. You don’t show the 2:00 AM computer sessions, or the scraped knees. Hopefully, it’s a challenge - but a respectful, encouraging, challenge - to @toothrobber that the effort is not only reasonable but worthwhile.


1 Like

Umm, ahh, errr, well maybe.

The initial motivation was my surprise when I posted a little earlier and found this:

I hereby certify that I am not simply asking someone else to design a footprint for me.

This is an auto-generated message that is in place on the “footprints” section of the forum. If I remove it and ask for a footprint to be designed anyway, I understand that I will be subject to forum members telling me to go design my own footprint or referring me to a 3rd party footprint site.

It seemed to me that it would be a pretty big surprise to the newcomer if a footprint was actually provided. Then, once I read the Datasheet to see what was involved, I felt compelled to help. The Datasheet only contains the drill diamter, and has no information on the finished pad size. Since PCB manufactures can be unclear about how the annular ring specification afffects the finished pad size, it just did not feel right to just let the OP continue to struggle.

But, yeah, once I made the mental decision that I was going to do this, I took note of the time on the clock. The intitial intent for posting the time was just to show others reading the forum that it just doesn’t take all that long to create a new custom Footprint with KiCad; but I won’t deny the possibility that the neatherderthal portion of my brain was trying to show off.

Great! Now I can call you Grandpa! :slight_smile:

Pretty sure there are more than one Grandpas’ regularly contributing on this site.

Maybe you should call @dchisholm Grandpa No.1! :slightly_smiling_face:

So it is a “Semi-SMT” or “Hybrid-Switch” or just a “Confused Switch”? :slightly_smiling_face:

Probably done for consumer products with a single sided PCB withe the switch on the component side.
I frequently come across the THT version on single sided boards, doubling duty as a wire jumper as well.
The first place I look for dry joints when I see these