Creating a footprint for a PCB

When I create a footprint for a through hole device to be soldered on a PCB, how much clearance should I allow for the lead? For instance, the data sheet for one device shows the leads to be 0.84 +or - .05. What size should I create the mounting holes on the PCB? Should I use the same clearance for all devices, or should they be a percentage of the lead?


Hello Bart,

I don’t know the specs, but the hole should be larger than the pin. Makes it easier to install the part, and gives room for the solder to flow in, and make a good connection. A lot of the through hole parts will have a recommended board layout, which includes the spacing and the hole diameter, on the datasheet. Maybe one on the engineers know of a tolerance or clearance dimensions, and can add to this post.

The specified plating thickness of plated-through-hole of a DKRed 2 layer board is 1mil ( 0.0254mm ).

This is going to be plating material that lines in inside of your plated through hole connections. You have to factor this thickness and make the specified drill hole this much larger than the hole that is needed.

To calculate the size of your drill hole you need to account for both sides of the diameter of the hole so you’d need to add 2mil ( 0.0508mm)

Which, adjusting for your lead(pin) tolerance means you need a diameter hole greater than 0.89mm + 0.0508mm ( 35mil + 2mil )

If it were me I’d make that drill 1mm or greater. 1mm is cutting it close due to tolerances.

Is 0.84mm the length and width of your lead?

Because in that case the hypotenuse of the right angle would be 1.188mm, which is the diagonal dimension of a square pin with 0.84mm x 0.84mm thickness.


Typically, the hole size on the PCB should be slightly larger than the lead diameter to allow for easy insertion during assembly and to accommodate any manufacturing tolerances.If the lead diameter is 0.84 mm, you might consider using a hole size of around 0.95 to 1.0 mm. Here is a detailed tutorial on how to create a footprint in Kicad.

The number of variables that go into determining the best hole size versus manufacturing technique are many. (e.g. lead diameter, PCB thickness, required position accuracy, lead stiffness, type of lead forming, type of assembly, assembly crew/machines)

There have been very few boards I’ve laid out for work since 1980 that didn’t need at least a few hole sizes adjusted, up or down, based on the prototype and/or first assembly run. Often the changes are only 0.1 mm (4 mil, .004") but ease assembly significantly.

The advise above from everyone else is very good, just don’t worry if your first build has you reaming out holes or clamping a part to accommodate too large holes during assembly. You can fix them all easily for the next PCB revision.

1 Like