I am trying to get a plated-thru-hole, used as a mounting hole, to be like a via in that I want to connect it to a filled zone, in this case a ground plane. On the schematic diagram I had the plated-thru-hole symbol attached to ground and when I went to my PCB layout it used thermals. If I put the no connect symbol on the plated-thru-hole symbol then on the PCB layout there is a gap to the ground plane. How do I get a solid connection, like for a via?
Also when trying various things I had a keepout area on my filled area ground plane that I deleted, but after refilling the keepout area was still there. I had to delete the filled area and redo it. Is this an anomaly or is this they way it works?
–Larry
I’m not looking at KiCad right now, but check the pad properties of the footprint you are using on the board. There should be somewhere about zone connection. You want a solid connection to zones.
Then hover over the hole, press "f"ootprint / [Select] and that will bring you to the Library Browser. Select a nice mounting hole from the “MountingHole” library and you’re done.
Tip: The via’s in the pads prevent the copper from getting ripped of the board. These mechanical vias are also very usefull for the mechanical pads of SMD connectors or when you want to solder thick wires directly to the PCB without connectors (For example with an ESC = Electronic Speed Control, used in remote control devices)
Edit:
After re-reading and a bit of experimenting I think you are looking for:
1). Hover over your mounting hole pad in Pcbnew.
2). “e” -dit
3). Pad Properties / Local Clearance and Settings tab.
4). Connection to Copper zones / Pad connection: [Solid]
5). “b” to regenerate the zone outlines.
In my Pcbnew (KiCad V5.0.2) the thermal spokes of the pad vanished, but it appears that all the via’s in this pad have their own thermal relief spokes. It looks like:
Thanx for finding it for Larry when I was too lazy to find it.
@9V1MI This is exactly what I was referring to. Watch out for the funny interaction if you have multiple pads overlaying each other and only change one to solid zone connection.
Yes, that did the trick. Changing the type of connection to solid was the thing to do. However, clicking on “Show filled areas in zones” or clicking on “Do not show filled areas in zones” and then “Show filled areas in zones” did not render a solid connection. I had to delete the zone and redo “Add filled zones”, then it showed a solid connection. I am using KiCad 5.0.2 on my Ubuntu 18.04.1 LTS OS. Is this the way it works or is this an anomaly (bug)?
–Larry
I do not see a reason for deleting a zone and redrawing a new one, unless the outline is completely wrong.
(Almost?) anything about a zone can be edited. You can edit the outline by inserting and removing corner points. You can move the corners around.
When you select a zone by clicking somewhere on it’s outline and press “e”-dit, you get a popup with the properties of your zone.
It also has options for the default thermal reliefs of pads. In the previous posts the defaults were inherited from the zone, If you want to edit all thermal reliefs instead of just some mounting holes then you should edit it here.
This does not regenerate the zone boundaries.
Regenerating the zone boundaries can be done with shortcut key “b” in Pcbnew.
Did you do that before delating the old zone?
You can also set this in the pad or footprint properties. This allows you to keep thermal spokes for all components that you solder but have the solid connection for your mounting holes.
I don’t think I used the Hotkey “B”–“Fill or Refill All Zones” as opposed to clicking on the icon “Show filled area in zones”. There seem to be a lot of these gotchas or nuances that are only learned from use and experience. Thanks for the information.
–Larry
