# How can I make a plated-through hole in Eagle?

I have mounting holes (0.125 in) at the corner of my PCB project in Eagle, made with the standard "hole" tool. However these are not electrically connected to anything.

There doesn't appear to be a way to make these plated through by specifying a net (unlike a via).

If I want my mounting holes to be connected to the ground plane, do I have to just make an oversize via? Is there some other way?

-

No, you don't want just a oversized via. Step back and think about the problem a bit. You don't just want a mounting hole, but rather a genuine electrical part. This part should show up in the schematic, be something you place on the board, have a pin connected to a net, and a pad that connection can be routed to, just like other electrical parts.

The correct answer is therefore to use such a part. This would have a schematic symbol with one connection. The package would be a thru-hole pad with the hole size matching your mounting screw and the pad diameter a little larger than the screw head diameter. If you want this to be a ground connection, connect it in the schematic to your ground net.

I have done this before and have a few such mounting hole parts in my library, including one for a #4-40 machine screw.

-
Agree 100% - in fact, the holes are precisely for a #4-40 machine screw (it's like you read minds). So I now need to evaluate whether Eagle has any such parts in its libraries, or if I need to create them myself. (I haven't ventured into library editing and device creation yet.) – JYelton Dec 5 '12 at 17:33
Followup: There is indeed a holes library in Eagle, as per @apalopohapa's answer (thanks!). I was trying to find a tool rather than a part; this is what I was missing. – JYelton Dec 5 '12 at 17:41

If I remember correctly, Eagle comes with a library called holes.lbr, with many plated hole sizes that you can place on your sch/brd, or use as template for a non-std size.

Those parts are basically a single through hole pad with some layers used to establish proper clearances.

Connect in your schematic to whatever you need the plating to be electrically connected, such as ground.

-
I think Olin's description of why one want such a part (instead of a via), combined with your pointing out of the holes library, is precisely the answer. (There is indeed a holes.lbr, thanks!) – JYelton Dec 5 '12 at 17:38

Oversized via is correct. If you want the throughholes to be connected to the ground net (plane), type via 'GND' 100mil or whatever your ground net is named and whatever diameter you want the copper surrounding the via to be (for hole size you need to first type CHANGE DRILL diameter with the desired hole diameter). You can also just click on the via button and select the various values from the drop down menus and change the via net name to your ground net with the name button.

-
+1 for simplicity, no "parts" to be added. – Anindo Ghosh Dec 5 '12 at 8:55
@Anindo: No, this is not a good idea. It may seem simple, but you are really working around the facilities in Eagle for this instead of using them to their advantage. – Olin Lathrop Dec 5 '12 at 13:04
the real drawback to doing this is if you do a "ripup", then vias created in this way will vanish without warning and you'll have to put remember to put them all back where you had them. It's dangerous stuff. – vicatcu Dec 5 '12 at 14:46
I was routing a board yesterday; I needed the ground pour to be ripped up for a moment and I didn't want to go find its edge to use the ripup tool on its edge. So I thought "I'll just type ripup gnd and that'll do it." It did indeed. Sometime later, I realized all of my ground vias were also gone, and it was much too late to "undo." So I totally agree with @vicatu. – JYelton Dec 5 '12 at 17:35

An oversize via will do what you want. The other thing you can do is to have a premade part with a single plated hole of a specific size and an appropriate keepout area for the screw head.

-