How to create complex copper shapes in Eagle

Question

I'm new to eagle but for a project I need to create a pcb with a complex arrangement of exposed copper contacts. The board is going to be used as a simple touch sensor made up of concentric and radial slices with each slice connecting to a separate pin (a sort of chopped up bulls-eye pattern). We're making the board on an LPKF pcb router which takes in a gerber file generated from a cam file it provides for eagle.

Whats the easiest way to "draw" these kinds of shapes into a copper layer? Thanks!

Answer 1

You can import vector designs from DXF file into Eagle with the help of this ULP script: http://todbot.googlecode.com/svn/trunk/eagle/import_dxf_polygons_v4.ulp

[no connection with the author of the script, found it this morning, worked fine for getting a simple design from Illustrator (exported as an R13 DXF) into Eagle]

Answer 2

As you can see here, I was successful in creating a copper layer using some obscure shape as the source image. Pragmatically speaking, the design is simple, but it could easily be more complex.

Here is the original image:

I created the image arbitrarily in MS Paint, and saved it as a Monochrome BMP image. This is important, make sure it is Monochrome (ie two colors only).

Then I opened up my library in which I would like to create the part with the obscure contact point. Create a brand new "Package" and then run "import-bmp.ulp". It is a sort of macro that comes with EAGLE. To run it, simply type "run", and you'll be brought to the directory of ulp's. Find the import bmp one and follow the procedure.

Only select the black color when moving through the wizard.

While following the procedure, you'll be presented with an option to set which layer you want the image to be imported as. You can make it one of the copper layers here, or perhaps a silkscreen layer or whatever else.

From there, you could set a pad in the center of the image so that you can have a pad to wire to in your board layout. EAGLE will not recognize your image as a pad so that's why you add the additional pad in a clever place where it will not screw up your design, but so EAGLE knows what pin/pad whatever, that your schematic needs to connect to.

Best of luck.

Answer 3

I believe the only One way to draw such shapes in Eagle is to use the wire, circle, arc, rectangle, and polygon tools.

Once you have drawn your desired shapes, modify the properties of the shapes to be on the appropriate layer. For a 2-layer board, they will be "Top" or "Bottom" layer. After, they should be the same color as the signal traces on that layer. Then use the name tool to change the name to the appropriate net for which you want the shape to be electrically connected.

When you first draw the shapes, they will not fill with the color of the layer and will have a dashed outline. Not until you hit the "Ratsnest" button will they become a solid color, better showing how they will appear on the finished product. Once the net is named correctly, any components located in the shape/plane will be automatically connected once the "Ratsnest" button is pressed as well.

Note that this is the same process as creating a ground fill if you need to search for more tips.

Edit: Per Olin's comment, to make my answer more clear, this is only one way to create complex copper shapes in Eagle. investingating the scripting capabilities of Eagle could alleviate reliance on the GUI icons.