MountingHole_2.2mm_M2_ISO7380
_Pad_TopOnly <-- I think this one only has a copper pad on the top
MountingHole_2.2mm_M2_ISO7380
_Pad_TopBottom <-- I'm not sure what the difference is between this one and the next
MountingHole_2.2mm_M2_ISO7380
_Pad <--
MountingHole_2.2mm_M2_ISO7380 <-- I think this one is just the hole with no copper pad
I think the difference between the second and third variant only matters for multilayer boards. The regular "pad" (the third one) also has pads on all inner copper layers, while the "pad_topbottom" has them only on the outer layers. So when you use a pad with a connection in your schematic, e.g. for grounding, a plated through-hole can connect either just the outer layers or the internal layers too.
You can study the footprints in KiCad's footprint editor to see how they are set up in detail.
The easiest way to compare differences is to just put them all on a PCB and then look at them in KiCad's 3D viewer.
[Edit]
In this particular case however, there is not much to see in the 3D Viewer. All 4 variants have are a Non Plated Hole, and the main difference seems to be the size of the graphical cirles around it.
I'd assume they become plated through-holes if you use them with a symbol which has a connection to the pad(s)?
Oops, I goofed up a bit with my previous post.
Screenshot is of mounting holes without pads.
If you do the same with mounting holes with pads however, you can see and compare where these footprints differ.
@ebastler:
Almost.
I assigned the footprints of my first screenshot from schematic symbols without pads for the mountingholes, and the (configurable) filter in cvPCB filtered out the pads with copper.
A good way to search through footprints is with the footprint browser. It has a "regular expression like" search function, and when seeking for "hole" and "2.2" (just a space between the two) Then you see 17 footprints for a 2.2mm hole:
MountingHole_2.2mm_M2_ISO7380_Pad_TopBottom <-- copper pad at the top and the bottom layers.
MountingHole_2.2mm_M2_ISO7380_Pad <-- this one finds use in the multilayer PCBs from my view where pads are throughout the holes.
the best way to understand this type of hole is by placing all of them on the PCB layout sheet and checking on its 3D viewer.
MountingHole_2.2mm_M2_ISO7380_Pad_TopBottom <-- copper pad at the top and the bottom layers.
MountingHole_2.2mm_M2_ISO7380_Pad <-- this one finds use in the multilayer PCBs from my view where pads are throughout the holes.
the best way to understand this type of hole is by placing all of them on the PCB layout sheet and checking on its 3D viewer.
Hmm... How does the 3D viewer show you what's happening in the inner layers? (Which is where the only difference lies between the two types of hole you refer to, in my understanding?)
If you turn off
Show solder mask layers and
Show board body then you can see the inside of the PCB.
Neat, I never tried that before.
But when I display a 4-layer board with these options, the viewer still seems to render only the outer layers (and the plated through-holes). The inner layers do not show up at all, and I did not spot another option to select which layers to display. Am I overlooking something?
Zoom in, WAY in. Look at the board from the edge.
That's what I did, but I don't see the two inner layers (Vcc and GND)?
When I make a plane layer by adding a filled zone that covers the entire board, the copper does not show up in the 3D viewer. However, the rings around vias may or may not be there depending on how I have the via configured. When configured as shown below, the annular rings do NOT appear in the 3D viewer.
The following is my findings for KiCad 5.
@ebastler make sure you have the inner layers enabled in the pcb editor, otherwise they aren't shown by the 3d viewer.
In the attached picture the left mounting hole is of the "_Pad_TopBottom" whereas the one on the right is "_Pad" only.
As can be seen, it doesn't affect if the pad is connected to the concerned net or not, but rather if there is a pad on the inner layers or not (as others have mentioned).
If you try to route around a "_Pad_TopBottom" on an inner layer, you can route in the area between the pads, but this is not the case for a "_Pad".
I'm not sure what the point of the "_Pad" footprints is though - improved mechanical strength?