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)

Through hole resistances
Through hole non-polarised capacitors

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)

1 Like

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

1 Like

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).

1 Like

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?

1 Like

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.

1 Like

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.

1 Like

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.

1 Like

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:

1 Like

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)


Hello guys!

@paulvdh I couldn’t follow your advice unfortunately, as i have not yet designed the pcb. So i couldn’t print it.

@jmk I went to your route and the resistors i have, fall under two catgegories (regarding their size).

These two categories are:

As far as the capacitors go, there is only one type i think

NOTE: Another set of caps i have is this one ( As you can see, the terminal pitch is the same. I am just adding this, because i do not know if terminal pitch is the only factor i should care about, but it is the only info provided by the page. There are no datasheets for the capacitors as you can see unfortunately…

For typical small elements (and hand soldered) it is probably the only important factor.
But in general the pad/hole sizes are also important. Hole can’t be too small to insert element legs. Too big is also not so good.
The CrtYd rectangle around pads also should be well fitted to allow you to not think about real element dimensions during PCB design. You just know - if CrtYd don’t overlap than I will be able to assemble them.
I use only elements from my libraries. When defining my symbols I attach to it the right footprint and never, ever go through step of footprint assignment.

I still do not know what to select, after the plethora of footprints offered by KiCAD…

  1. Select a few footprints you think that may work in Eeschema.
  2. Put them on the PCB with [ F8 ]
  3. Do the test fitting I described in my first response.
  4. Iterate until you have all footprints.

Remarks like:

do not help. You can keep on doubting untill the cows come home, and they wont. Just try some, and see if it works on a test print. Such a test print is easy and quick to make. If you then get into trouble with a footprint you can ask a more direct question.

Over time you will build up some experience and it will become easier.

All the footprints in KiCAD have three sets of numbers (and mm units next to them).
What do these numbers mean?

I will do tour approach eventually.

I was thinking a more linear approach but it does not have to be.

the meaning of the numbers may change a bit depending on the exact part you’re looking at. If you look at the number earlier posted by Mr. Blitz:

  • L3.6mm = Length of the body.
  • D1.6mm = Diameter of the body.
  • P7.62mm = Pitch of the pads, center to center distance of the holes.

Rectangular parts of course do not have a diameter, and there may some other differences, but within a family the numbers should be consistent. Exact meanings are probably also explained in the KLC

Check out section F2 - General Footprint Naming Guidelines of the KLC (KiCad Library Conventions). The libraries for V5 were made to these conventions.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.