Archive of the former Yahoo!Groups mailing list: Homebrew PCBs

After messing a bit with ground planes, isolation etches, and copper pours
with Eagle Lite 4.15, here's a quick how-to:

POLYGON defines the outline of a copper pour. Drawn on a signal layer, 1-TOP
or 16-BOTTOM, they can be given a signal name. This signal is then
associated with the pour. The most reasonable signal for a ground plane is
GND. Other signals are separated from the pour by a specified ISOLATION
distance.

The "trick" to doing this is to first ripup the traces on the layer with the
pour. I tried this (in vain, frustratingly) first on a board that was
already routed, thinking it should carve the bottom traces into the new
pour. This apparently doesn't work. Many long minutes were spent this way;
it felt like hours, weeks. I even gave in and read the manual. A root canal
would have been more fun. And then tossing caution to the wind (not really;
the file was backed up safely), I ripped up the bottom traces and gave it a
clean slate to work with. The simplest way to do this is to turn off all
other signal layers and ripup all the signals. (Semi-colon does this nicely,
automatically.)

Draw the polygon outline with a reasonable width; I used 16 mil, wide enough
to see easily, and narrow enough to select easily. This is only the outline;
Eagle fills in the closed shape. (Later, of course, so you wouldn't know
what to expect...)

Set the ISOLATION distance in the toolbar, or use CHANGE ISOLATION later. I
used 16 mil. If you're milling this, maybe use the end mill diameter. The
default distance is 0, not very useful for a ground plane.

Draw a box around the dimension extents. Polygon segments must not overlap
or cross each other. I even got Eagle to crash completely more than once by
screwing this up. The best way to do this is to trace three sides of the
bounding box, and sorta click twice on the fourth corner, but not quite
double click. You just want to click the same point twice without moving the
cursor. Eagle closes the outline back to the starting point, drawing the
fourth side.

Now run the auto-router. I didn't try routing manually, so I don't know if
that works. I expect it should. The POLYGON is calculated by RATSNEST or by
AUTO. It stays an outline until either command is run. After it runs, the
pads and vias are isolated, and new traces are properly isolated. Existing
traces are apparently not examined by RATSNEST; they remain untouched and
unisolated.

Ground pads are connect to the ground plane through thermals, a very nice
touch. Thermals are small traces through the isolation space around the pad,
connecting it electrically but isolating it thermally so it can be soldered.
I think you can specify how many and how wide in the design rules; I always
wondered where that was used. Now I know. :) And now you know. Have fun. It
really cleans up the ground traces nicely.