Hi, could somebody tell me how I can design drill holes in PCB? Up to now I have created pin headers in schematic, but I wonder if there is a way on pcb-level.
Drill holes up to 6.35mm (1/4") are best defined by footprints that are drill holes without anything else, examples:
Plated Trough Hole:
z_MountPTH_3mm.kicad_mod (688 Bytes)
Unplated Through Hole:
z_MountNPTH_3.0mm.kicad_mod (690 Bytes)
Anything bigger than that should be defined as circles on the outline layer as it will be milled in 99% of the cases.
If you define holes on the outline layer with a diameter less than 6.35mm expect +/-1mm final diameter error at the more economical fabs.
Also keep in mind that there is just a finite number of drill sizes available at the fab. Your boardhouse will usually round up/down to the nearest 0.05mm size for drilling (this also applies to vias).
I think what KiCADsmktec is asking is does each footprint (especially for drill holes) need to be in the schematic. It does not. You can have extra footprints on your board that aren’t in the schematic. To do this you always have to select “Extra Footprints > Keep” in the Netlist dialog when up update the netlist. This also happens to be the default option. You add the holes with Place > Footprint. The holes do need to be a footprint, but there are some generic ones in the Mounting Holes lib that comes with 4.0+ stable.
That said, I like to enforce consistency between the parts listed on the schematic and board. I have a simple mounting hole schematic symbol that I use for any size hole and I also create logo symbols to go with the footprint. Having these items on a schematic page dedicated to mechanical items is pretty common in industry.
I don’t recall ever seeing a SCHEMATIC that contained mechanical information such as hole sizes, logos, etc. I also like to have “clean” documentation packages that don’t trigger nuisance squawks from the DRC/ERC tools. Having all that mechanical information on the schematic would probably strike me as distracting from the intent of the drawing, though others may see it as inconsequential or even helpful in some way. I just wish that KiCAD had a way to add sheets to a schematic without going to the complexity of a hierarchical drawing.