Thrilled with Eagle EDA

Oops. Good catch.

I phrased that poorly, indicating that I had autorouted over the planes rather than what I actually did, which was autoroute, disconnect the Vcc and GND nets and *then* applied both the Vcc and GND planes.

I was trying to communicate that the 'Vcc' and 'GND' connections automatically connected themselves to the proper plane (after 'naming' the plane, doing the obligitory 'ratsnest' command and connecting vias where necessary. There was a little additional cleanup involved in managing current flow, but I am still astonished how easy that process can be.

I let my enthusiasm get in the way of clarity there.

--Winston

Sure is, I played with the polygon and nothing useful came out of it, can you put a demo file up somewhere?

Or describe a command sequence that will let me see it work? I've read the polygon command is the right one for filling or pouring copper.

Grant.

This guy did a far better job of it than I could've:

The only difference is that in the fifth picture down, I type 'rats' in the command line box to make the plane visible, because the solid fill does not appear after 'naming' it, at least for me. On opening my file for example, I notice that the planes are never visible until I've typed 'rats'.

Here is a time-saver. When you want to edit your board after having poured one or more planes, type 'show' and click in the border area where you first outlined the plane. After one dotted outline 'highlights', type 'rip' and click on that border once more. The plane will revert to it's 'outline' rather than 'filled' appearance. Don't panic! You have *not* lost your plane.

Repeat these two steps for each plane on your board. Note that it is *not necessary _or_desirable* to _delete_ any plane's outline border if you are happy with the outline geometry. After editing your board, just type 'rats' again and your planes will be re-generated *including allowance for your edits*.

It is magical to watch, IMHO.

Let me know if you run into difficulty with this.

--Winston :)

If your plane's dotted outline does not show up, right mouse click in that border and click on 'next' in the resulting dialog box until the dotted outline does appear.

if you turn of orphans on the plane the unconnected islands will disappear making it easy find them

-Lasse

Eagle EDA does have an unattractive feature. Running the CAM process produces results that has a random X,Y offset added to the real numbers.

Here is my workaround:

Make sure your entire design is located +X and +Y (above and to the right of) the little '+' fiducial on your screen.

In your source file, place a 0.001" hole at some obvious location on your board near the lower left corner. I shall use X 1.0, Y 1.0 for example.

Run the CAM process to generate your Excellon drill file. Remember to manually add the '.txt' suffix to your suggested file name for results and remember to click on the dialog box *twice* because you are processing both 'pads and vias' and 'holes'.

Open your Excellon *.txt file and find your 0.001" dia hole within. Note it's location.

Run the CAM process once more and edit the 'offset' variable to cancel the offset in the results file. Recently, for example, I cancelled their error when I plugged in an offset of X = 0.0010", Y = -0.0151". The 'Y' offset will eventually show up as a metric value while the 'X' offset will remain in olde englishe inches. It's a feature. :)

Run the CAM process again and confirm that your 0.001" hole is now shown at X = 1.0000, Y = 1.0000 in the Excellon file.

After every few edits, run the CAM process again and adjust your offset as necessary to bring your 0.001" hole error back to zero. Make note of the location of a nearby 'real' pad or hole for future reference.

Just prior to generating your real CAM files, delete your

--Winston

(...)

Cool! Thanks.

--Winston