drew keller wrote:
I am mounting a PCB to a transformer that has quick terminals on it. So
I am trying to create a library part that has slotted through hole pads....
I created the slotted pads in the package by drawing thick WIREs in the
pads layer and thin WIREs in the milling layer. But when I try to bring
the package into the device definition, there is an error that says
there are not enough pads to match my symbol.
Maybe there is a better way to do this.
Thanks.
-drew
You never created any actual pads that EAGLE recognizes. EAGLE makes a
distinction b/t places where your are just defining metal and if a
defined area of metal is a pad meant for electrical connection in a
netlist.
What you should probably do is:
-Create the slot in the Milling(46) layer.
-Add an SMD pad to either the Top(1) or Bottom(16) layer.
-Draw a polygon of the same shape as the SMD pad, and place it on the
opposite layer.
-When you CAM-up your .brd file add an extra section, call it MILLING,
set the extension to .mll, select the Milling(46) layer and process the
entire job.
-Tell your board house that the .mll file has information on milling
that needs to be done before metallization.