NPTH Mounting Holes ... AAAaarrgh! Or, how to get them right the first time

Layout
22

I never understood what should be confusing with them. They are used like any other pad inside a footprint. (And added to your board like any other footprint)

I think you mainly hang yourself up because you do not want to use symbols for such things. This is understandable. But any additional complications that arise from this fact are for you to deal with.

Maybe a better tutorial for adding mounting holes is as follows:

Step 0: decide if you want to have symbols in the schematic or not. (Suggestion for new users: use a symbol. Makes everything easier.)
Step 0.1: decide if you want plated or non plated mounting holes. (determines which symbol and or footprint to select)

  • Plated holes allow more mechanical strenght.
  • Plated holes can be used to connect ground to your housing

With symbol in the schematic:

  • Add the mounting hole symbol found in the mechanical lib to the schematic (either the one with a pin for plated mounting holes or the one without for non plated)
  • Annotate the schematic.
  • Assign the footprint for your mounting hole to it (the official lib comes with quite a few mounting holes. If you need more then create one. more on that later)
  • Save your schematic and switch to pcb new.
  • Use tools -> update pcb from schematic to get your stuff into this tool.
  • place the mounting holes like you would any other footprint.

Without symbol in the schematic:

  • Add the appropriate footprint with the add footprint tool from the right toolbar.
  • place it where you want it to be.
  • Lock the footprint to protect it from being removed by updating from schematic. This is done in the preferences menu of the footprint (Important: The preference menu of the footprint not the one of the pad!)

Creating a footprint for a mounting hole

  • Create a new footprint inside a personal lib.
  • Add a single pad to it.
    • Choose either plated or non plated through hole depending on your needs.
  • Add some indicator for the size of your screw or other part to the fab layer
  • Add a courtyard layer with enough clearance to the screw (depends on your needs/preferences.)
  • Save the footprint

More details about footprint creation: Tutorial: How to make a footprint in KiCad 5.1.x (From scratch)?

3 Likes
23

Hi All

I would suggest in PCB_New, try a brief test or inserting EVERY mounting hole for size M3. Then look at the PCB using the PRINT BOARD (icon of printer) and be sure to make each layer a different sheet. In Preview you’ll see which are just drilled, which have an annular ring, extra GND holes, etc. You’ll quickly pick a favorite and stick with it.

Regarding “professional” schematics/pcb, particularly in RF and microwave, it is often necessary to have a Really good Gnd so there will be instructions like “provide a Gnd mounting hole within 0.2” of Q2 emitter". The same for stitching Gnd planes on both sides. These tidbits are essential to proper operation and in 10 years when the board is revised, it is extremely helpful to have this knowledge.

It is a very quick and useful learning experience. Also learn to LOCK mounting holes after placement or they may wander on you.

Keep learning and good luck!