Creating PCBs in Eagle is a straight-forward process once you understand how EAGLE works. In fact, most users can get up to speed enough to draw a Schematic and then layout a simple PCB. Making the connections between components is not only fun but can be a form of artwork.
Often overlooked is how much space is left wide open. For example, a board might look like this:
The area in black will have no copper. For circuits that don’t require a ground plane, this may not be an issue. However, it rarely hurts to fill in empty area with a ground plane. EAGLE makes it very easy to do this, after your circuit design is complete.
Step 1. Create your PCB
My suggestion is to not worry too much about how to fill your empty spaces with a ground plane. Simply lay out your board as cleanly as you can. [Note. This advice is for low-frequency circuits with content well below 1MHz. For high-speed layout, certain rules must be used.. So, lay out a board.
Step 2. Draw a Polygon
Once a board has been designed, using the POLYGON command, draw a rectangle (or whatever shape you wish) around the perimeter of your entire board. Do not worry about holes, but you should follow your (20) Dimension Layer if you have an unique shape to your board.
Step 3. Give the Polygon a Name
Right now your new POLYGON has a NAME that EAGLE has assigned to it. Change the name of the POLYGON to GND using the NAME command. When prompted select “this Polygon”.
Congrats, you have just created a ground plane, isn’t it beautiful. Wait, something is wrong. The board looks like it did before. Hm. EAGLE will not fill in the POLYGON until you run the RATSNEST command. So click that now. And ta-da we see a ground fill in the printed circuit board.
EAGLE will not fill in the POLYGON until you run the RATSNEST command.
Step 4. Isolate!
There doesn’t look like much space between the traces and the ground plane. This might cause issues when manufacturing the boards. So let’s increase the isolation area a little bit by using the INFO command. Personally I like to use 0.016, but your mileage may vary. If DRC gives clearance issues, increase the Isolation a little bit.
While in this window, make sure the “Thermals” box is checked. This box will give some thermal relief around ground pins and vias that connect into the plane. Without this thermal relief, it will be very difficult to solder to the pad, since the ground pour will act as a huge heat sink.
Step 5. Don’t forget the top layer
Now go back and repeat steps 2-4 for the top layer.
Step 6. Add some Vias
One of the important things about having two ground planes is they need connection points. So sprinkle a couple of Vias around the board and change their NAME to GND. On through-hole boards this is less important, but always helpful.
Exercise for the Reader
Doing these simple steps before generating your Gerbers will result in more professional looking boards, and in some cases, may even result in a most robust PCB design. Something I like to do on my boards is to keep the bottom layer’s POLYGON solid while making the top layer’s POLYGON “hatched”. This is done in the Properties window (INFO command) and selecting a different type of Polygon Pour.
Question: The “Run Ratsnest” is a critical step here. What else has tripped you up in EAGLE? You can leave a comment by clicking here.