I do this two different ways, but both end up with a schematic element.
I don't like PCB-only elements because I regularly re-import and change
netlists during layout , allowing modules to change and be deleted.
The technique I use most frequently is to use the CONN_1 module in the
schematic and specify an appropriate footprint. I have footprints for a
range of SAE and Metric mounting holes with large and small washer
profiles. All are plated through. The CONN_1 module usually ends up
connected to ground or a no-connect. I put "Mechanical' in the
description field and use that to strip them from the BoM. I do the
same for jumper patterns that don't actually mount parts. One mutlisheet
schematics I usually put these on a separate and last page along with
things like stitch vias and overall notes.
The alternative I use is to build a board outline and hole pattern in a
footprint. This has the disadvantage of making DRC go nuts because you
are putting parts on top of parts. It has the advantage of a cleaner
schematic and automating the process for common outlines like those that
fit in packages or mount a daughterboard like a Raspberry Pi.
As a variant of the second option I have a number of footprints that are
only on the edge, drawing and silkscreen layers. These have drawing
layer targets for connectors and holes as well as silkscreen for
outlines and label text. I have a few I've done that include mating
connector footprint elements, but I prefer having the connector as a
discrete item for the BoM.
As to plated vs not, I /almost /always use plated, isolated pads instead
of non-plated. In the rare cases I've need non-plated I check with the
vendor and determine their preference. In the case of Oshpark this is
specifying copper smaller than the hole size. I've done the same thing
with Elecrow and they'd not complained. My readme file explained what I
was doing. I needed unplated holes for the guide pins of a modular
(aka RJ45) connector. I did plated slots on the same board using the
oval hole option in the pad description.
Oz, in DFW
Post by ***@arius.com [kicad-users]Someone earlier said they added mounting holes to the layout without
adding them to the schematic. So I guess they become 1 pad
components. I prefer to include *everything* on a layout in the
schematic. That makes it easy to run a check to make sure the layout
and schematic are always in sync. Adding mounting holes to a
schematic is not a terrible idea anyway. They often serve as
connection points to the chassis ground.
Rick
--
mailto:***@ozindfw.net
Oz
POB 93167
Southlake, TX 76092 (Near DFW Airport)