Turn your EAGLE schematic into a PCB

Step 13: Add power plane polygons

"Power planes" are large areas of copper that carry an actual signal, usually power and ground. On multi-layer boards, it's common to have entire layers mostly dedicated to such a power plane. Even on a single layer board there are some advantages to doing something similar:

1) Use less etchant
2) carries heavier current, just in case
3) makes it easier to attach test leads
4) acts as a sort of "static barrier" to fingers

In EAGLE. such large signal areas are drawn with the "polygon" command. There is an icon on the toolbar for drawing polygons, but it will create polygons associated with a new signal, and I find that when creating a polygon for an existing signal, it's easier to type the text form of the command in the text command area. To create a polygon attached to a signal named 'gnd', type "poly gnd" By giving it a signal name in the command, the polygon will automatcailly be connected to that signal. (If you draw a polygon with the icon, you can connect it to a signal later by using the "name" command to rename the polygon. (however, after this, you can't rename the polygone again without renaming the signal as well.))

Comments

[alr206]

How do you get it to incorporate contacts that are connected to gnd? Everytime I try, it excludes those areas (I am using your design rules file). Thanks -- your instructables have been VERY helpful!

[westfw]

make sure that both the signal and the polygon have the same name (ie "gnd") The easiest way to name the signal is to attach one of the "gnd" symbols to it, and for the poly it's easiest to use the "poly gnd" to create it, but you can also name them with the "name" command/button.

[abraxas2]

Every time I try to rename a signal path or pad, in board view, it says "Cannot Back Annotate ...Change in Schematic View" So after many attempts I finally manage to change one of these items names to "Base" , in schematic view, since it connects to a transistor base. It prompts me with an invite to connect Base and Gnd, I respond "no". The adjacent signal path which I do want renamed gnd, keeps on resetting to the name Base and won't let me change it to gnd...no matter how many times I try. Worse yet, when I do the gnd plane, both the Base and Gnd signals get tied to the plane. It's driving me nuts.

[abraxas2]

The only thing I can see is that I have some very faint phantom lines connecting the Base and GND traces. These are lines I believe left over from a Rip Up repair. I'm guessing the program still thinks these items are connected.

[alr206]

I didn't realize that what I actually had was thermals, so the pads should appear a little bit different under a closer view than in the pictures above. Thanks again!

[westfw]

Ah. Yes, I have thermals turned off in my init files, which makes my normal behavior different than the default behavior. I should be more careful about that!

[abraxas2]

I can't thank you enough for this excellent tutorial. I thought I'd never get the hang of it and it's not a very intuitive program. Do consider turning these tuts into a book. Now hopefully one last question : after drawing the ground plane with the ratsnest command I got a nice big plane but also a bunch of tiny little islands that serve no purpose but to make the board look dumb. I tried erasing these islands with the rip up but it just ripped up the closest vital wire instead. Is there away to zap these tiny little island ground planes ? Thanks MUCHO !!

[westfw]

you can draw lines and/or rectangles in the tRestrict or bRestrict layers, which will prevent the polygon fill from entering those areas. You can see this in the PCB that goes with http://www.instructables.com/id/Single-Sided-Really-Bare-Bones-Board-Arduino-in-EA/ - I use it to prevent copper between the pads of the bottom-side SMT capacitors. Note that the restrict layers are not displayed by default; you'll have to turn them on in the layer menu (they might get turned on automatically when you draw on them, too.)

[abraxas2]

It mysteriously fixed itself. Thanks.

[westfw]

(did I set some kind of record for time gap in between publication and "featuring" ?  About 3 years!  (To be fair, there was no such thing as "featured" back when this was first written.  It makes me wonder what other really good instructables are languishing unnoticed mostly because of their age...))

[joeuhlik]

Why does Eagle want to draw the polygon as line segments rather than as a rectangle as you show?

[westfw]

It'll draw the outline as per the current settings for line-bending and etc as specified for "wires"; to get a rectangle, I usually set the line bend to right angles and draw two "L" shapes.

[diyuser]

How would you tell Eagle not to draw polygons/power planes when auto routing. Just plain wiring.

[westfw]

I don't think Eagle ever creates polygons during autorouting, though it may use any existing polygons as THE route for whatever signals they represent.  I always end up spending a fair amount of time adjusting exactly how the polygons fill; I don't like the way it tends to create "spikes" in the areas between pads, for example.  It all has to be done manually.

[keithongrq]

i've done every thing here and the end result look good but when i save the file and reopen it, the polygon becomes a rectangle made of dotted lines. some help please thanks

[westfw]

This is normal. EAGLE doesn't "render" the polygon on the screen until you issue a "ratsnest" command. I'm pretty sure that gerber output would be correct anyway, and having the polygons displayed as outlines makes it easier to route additional tracks.

[jimmy dean]

When I try and draw a polygon, it's never filled in. When I finish the polygon it just makes a rectangle made of dotted lines.

[westfw]

Assuming the polygon is attached to the appropriate signal (it should contain a pad, smd, or via connected to the signal within its borders), it will fill in when you issue a "ratsnest" command.

[jimmy dean]

Oh, i didn't do the ratsnest, thank you.

[josheeg]

This part is super cool! I am making a board with power gnd and analog ground so I need 3 different polys and this helps reduce noise. Thanks