I have a vexing problem and I’m hoping there is a simple solution… I need to make a pad with an inside diameter of 19.5mm and an outside diameter of 22.5mm. Unfortunately, the largest pad diameter allowed using the Change command is 13mm so I set out to make my own custom pad. And that’s when I realized that I might be in over my head. My idea was to draw two concentric circles and then “fill” them, but how to get the through-hole plating? If this is not possible, it’s not a big problem, but I’d prefer to make this an actual “pad”, rather than a big hole with a ring of copper around it. Thanks for any help!
A hole this large will not be a drill, it will be an internal route. Please keep that in mind when choosing PCB manufacturers, for example BatchPCB won’t do it. You will have to specify the hole as copper and then a Mill path.
In my experience, if you don’t specify a hole to be non-plated, then it will be plated. You could make a ring or concentric rings, then make a circle Mill path that is within the edge of the copper area. This means the copper will “spill over” and make an electrical connection with the hole plating.
You may have to engage in some kludging during part creation and actual layout, depending on where you plan to connect any signal wires. I would be inclined to do this on the board, rather than on a part. That way, you could name the layers of copper the same as the signal you are trying to connect, and the airwire will disappear when an electrical path is created to any point on the circle.
Also keep in mind that routing is typically done as the last step of board fab; so make sure your board fab knows to do that before plating!
Thanks for the reply, macegr.
So is my idea of drawing two concentric circles and then filling the space between them viable? Two more questions: what layer(s) should I draw the inner and outer circles on and how do I tell Eagle to make the inner circle an internal routing, since it can’t be called a “drill” (and, well, it’s pretty obvious why now that you pointed it out!)?
Thanks!
I had boards made with my kludged huge pad and thought I would provide an update. Here’s a pic of the pad on the finished board:
http://tesseractcorp.com/pics/big-pad.jpg
Note the vias… I’m glad I put them in because the internal routing to make the big hole was done last, despite my instructions otherwise, so no through-hole plating to connect the top and bottom (or internal) layers together. on the plus side, the board-house I use (Imagineering) did correct the missing soldermask around the “pad”, an error that was the result of my kludged method of making it. I had to manually create the soldermask because as far as Eagle is concerned my pad is “dimensionless” - it was drawn as a single circle with a diameter of, e.g., 0.8 and a line thickness of 0.1 to produce an annulus with ID of 0.7" and OD 0.9". This works out just fine on the board, as can be seen, but Eagle still thinks of the circle as just a circle, not an annulus. Anyway, maybe this will help if someone needs to make a rotating contact (in which case you want to use gold plating, not solder).