Disclaimer: Screenshots taken in a nightly from after the 5.0.0-rc2 tag. (KiCad 5 will look very similar but there will be slight differences in KiCad 4)
Other FAQ articles worth reading:
- What is the difference between footprints and symbols?
- Creating a new footprint library
- How to check footprint correctness?
- What is the meaning of the layers in pcb_new and in the footprint editor?
Other interesting resources:
- Import/Create FootPrint DXF (Designing a footprint using freecad and a background image)
- Freecad sketcher tutorial
Creating a footprint using the footprint editor
All elements of a footprint are specified relative to the footprint origin. This means pads are defined via their center point relative to that origin plus size specifiers.
To create a footprint the first step is to translate dimensions given in the datasheet into a form that gives the center position and size of pads. (Relative to the chosen center)
What center should be chosen for the footprint?
If your footprint is intended only to be used by yourself and you hand populate the pcb, then you can put the center anywhere you want. (Make it easy for your self. We will get back to that later on.)
Center point for automatic assembly
If the pick and place center position is given in the datasheet then use that.
For surface mounted components (SMD) the center of the part body will be a good choice for the footprint center.
For through hole parts (THT) typically pin 1 is chosen as the center position.
Something important to keep in mind: If you plan on having your board assembled by a machine, talk to the guys programming it. They can give you guidance.
Getting dimensions for the footprint
Disclaimer: This section might go into too much depths for a novice. Especially the later subsections. In practice eyeballing the dimensions should be ok for a lot of use-cases. Especially true if the part is hand-soldered. It might still be a good idea to read this as it might give you inspiration for how to improve your skills.
What can be expected inside a datasheet
Every good datasheet at least contains a detailed dimensioned drawing of the component. Some even contain a suggested footprint layout to give the user a starting point.
Such a suggested footprint should not be taken at face value. Especially older datasheets might be out of date with current manufacturing methods and industry standards. (Meaning if you have access to some reliable piece of information that contradicts the suggested footprint, it might just be that the datasheet is wrong.)
The dimensioned drawings are most likely found somewhere near the end of the datasheet. (Not all datasheets follow that rule. I have encountered datasheets where the packaging information is somewhere in the middle.)
Some manufacturers do not include the dimensioned drawings in the datasheet but have them in a separate document.
What to do if datasheet does not give a suggested footprint?
If a datasheet does not contain a suggested footprint, it is possible that the manufacturer supplies an application note that aids the user in creating a valid footprint. Dimensioned drawings of footprints in such application notes do not necessarily apply to the component in question. (Application notes might be written with many different components in mind. Drawings might just be examples for some of them.)
Some conclusions can still be drawn from the application note even if it is not for the exact part you are using.
Another source for information are similar footprints from a trusted source. In most cases it is easier to modify such a footprint than to create one from scratch.
Datasheets of similar parts by other manufacturers can also supply some useful information. Especially if they contain both a dimensioned drawing of a footprint and the package. If the dimensioned drawing of the package is the same as your component then you can use the footprint as is. Otherwise you can use it to get information about fillet sizes. (More details in the example about the qfn footprint below.)
Some manufacturers also have a specialized tool with its own specialized file format to share footprints with their users. (Analog devices is an example for that. Sadly their tool only runs under windows. It also requires you to register with them. At least at the time of writing this.)
Using industry standards
Industry standards can be of great help when designing a footprint. Sadly such standards are most likely closed. (They are quite expensive.) One well known standard for smd parts is the IPC-7351 series. (IPC-7351B is the most recent standard at the time of writing. IPC-7315C is expected to be released soon.)
There exist tools that generate footprints in accordance to IPC standards. All of them however are closed and cost quite a bit. (If you really worry about being complaint this will be the price to pay.)
There are some open tools out there (Example: The python footprint generator for kicad has some ipc generators The QEDA project also has some IPC footprint generators.). Such tools are not able to give you a certificate for your parts.
We will discuss the terminology used in this standards later on. We will also design a footprint using some of the more easily to find recommendations. (With some patience a surprising amount of information about this standard can be found.) Older IPC standards can even be found complete on some file sharing sites. Be aware that sharing them would be a violation of copyright. (This is why we will not link to any such documents here.)
Talk to your manufacturer
If you know which manufacturers will be used to produce your PCB and also who will be used to solder it, you might want to ask them for their “Design for Manufacturing” (DFM) guidelines. These guidelines might contradict other industry standards. (Like with every other competing set of standards.) Use your own judgment what guideline to trust. (If it is critical it might pay to produce some sample pcbs and analyze the result.)