Figuring out what footprints to use

I am in the stage that i have finished my schematic and i have to select footprints for my components before heading over to PCBnew.

However, i could not find a guide on how to select footprints.
I am very scared of this part, because this is the most important part, if your components will match the footprints.

I got my introduction to KiCAD, through the ‘Getting to Blinky 5.0’ series.

The good part is that my parts are few and very basic.
On the one hand i have common resistances and capacitors, and on the other, arduino parts which i guess they are easy to find (if only i knew how)

COMMON PARTS:
Through hole resistances
Through hole non-polarised capacitors

ARDUINO PARTS:
Arduino power jack
Arduino button (it has 4 connectors)
Arduino pin headers (I need them so they are one next to each other - only two pin headers)

The through hole components are so common. It’s a shame i cannot pick one.

The resistor and capacitor THT footprint library have so many components with mm… I just need common resistor/caps you can get on any hardware store.

And about the arduino parts, they are very common.

If you could help me that’s awesome.
If you could point out a guide on how to select proper footprints, that’s great as well!

Thank you!

For resistors, I tend to use “Resistor_THT:R_Axial_DIN0207_L6.3mm_D2.5mm_P10.16mm_Horizontal”, which is a pretty standard 250mW device. (so should work for any modern resistor)

If you go for 125mW resistors, then use “Resistor_THT:R_Axial_DIN0204_L3.6mm_D1.6mm_P7.62mm_Horizontal”

For capacitors, it’s quite essential that you know what you are using, as size and shape can vary a LOT, depending on the type of capacitor you are using.

The 100n capacitors I use for decoupling nicely fit: “Capacitor_THT:C_Rect_L4.6mm_W2.0mm_P2.50mm_MKS02_FKP02”

My 220 / 470 nF caps are a bit bigger: “Capacitor_THT:C_Rect_L7.0mm_W4.5mm_P5.00mm”

I use fairly (physically) small capacitors, so use something like “Capacitor_THT:CP_Radial_D5.0mm_P2.00mm”

(If you are in UK, let me know what sort of R and C you are using, I get them from CPC, so could point you to some relevant part numbers)

Start by fitting some footprints that seem to work.
Then do this:

The official library gives the sizes of components in milli meter (this is true for every generically used package not just simple passives).

So the typical workflow is as follows. After or during drawing the schematic one selects which exact components to buy (most likely by searching the webstore of ones favourite distributor).


This typically means one now has access to a datasheet for every used component. These datasheets then contain dimensional drawings that one uses to either find out how the footprint shall look like.

For a through hole resistor you would look up the diameter and length of the main body (the pin pitch is mostly personal preference as to how much space you want to give yourself for bending the leads).

For a capacitor you will first need to know what shape it comes in (is it a cylinder with leads at oposite ends or at the same end, or is it a disc with leads exiting to the side or is it just a cuboid).

  • Cylindrical with leads on opposite ends are like resistors. You need body length and diameter to select the footprint.
  • Cylindrical with leads at the same end means you need the body diameter as well as the spacing (pitch) of the leads.
  • For disc style caps you will need the diameter and thickness as well as the pin spacing (be aware that not all such caps have the pins in line with the center line of the disc. So you might need to consider not just a pitch in y direction but also in x direction)
  • For cuboid you would need the size of the body as well as lead spacing.

If your distributor of choice does not offer datasheets or you feel unsure in how to read it then you can also just order a sample and measure it with calibers.

Having the component at hand of course also allows just printing the footprint 1:1 and checking it against the part (really only feasible for through hole components as the human eye is not precise enough to really check footprints for surface mount devices).

As you appear to be very new to this hobby it would be best for you to purchase the parts needed before you attempt your board layout.
That way you can measure the parts and then select the footprint that best fits.
You mention Arduino parts. Are these genuine Arduino parts or are they just standard pieces of hardware used in an Arduino project?

This is worth repeating:

THT Resistor leads are almost always bent to a 2.54mm grid. ( = 100 mil) You can put your resistor into a piece of matrixboard (or breadboard, (with sufficiently short cut leads)) and then count the holes.

The best way to browse through footprints is with the Footprint Editor:


and then use:
Footprint Editor / Inspect / Measure to get on screen measurements.

Thank you all guys, very helpful!

No, i mean my parts are the same that an ordinary arduino wears. The power jack, pin headers, and a button.

Hi Nick, you will almost certainly find all the parts you require at a bricks and mortar or online electronic parts retailer. Any push button switch, no matter what size or shape, provided it does as your schematic shows, will do the job. As I stated above, get your parts then sit down with a ruler, measure the distance between pins, measure the outside shape then find a footprint that fits. If you can’t find a footprint in any of the libraries, you will then have the opportunity to design one yourself. :slightly_smiling_face:

BTW, Paulvdh mention breadboards and matrixboards. In case you didn’t know, back in the good/bad/indifferent old days, most electronic parts were designed around 1/10th of an inch increments.
1/10th inch = 100mil = 2.54mm. Hence, Pauls’ reference.

Measuring the parts really should be a last resort. The better option is to get parts for which you also get a full datasheet including a dimensioned drawing. This cuts down on possible measuring errors and it also tells you which tolerances to expect.

If you don’t have the datasheet for your part, you should also do the measurement to make sure the datasheet for “similar” part matches dimensions of your component :wink:

There are several stock parts that are, basically what you want…

BarrelJack Horizontal is the Power Connector.

PinHeader_1x08_2.54mm Vertical (and other pin quantity’s)

SW_PUSH_6mm is the button switch and various height’s of button

Here’s a Tip: Use the Search-Field to enter a ‘word’ belonging to the parts name and, Double-Click one in the Footprint Panel and use the View>3D Viewer to see the part (if the 3D model exists)

1 Like