• Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

CadSoft EAGLE, complex custom pad shapes.

Not open for further replies.


New Member
Hi, how would one produce this custom pad shape, in eagle pcb designer. All I could find was a video of simple, 90deg polygon shapes.
The design is a cutout on pcb edge for a switch, the area needs to be filled. any solutions. thanks



Well-Known Member
Most Helpful Member
I am on the road with only Android so no Eagle CAD. It looks like this switch is on the edge of the board!
I would try a rectangle pad.
1) place the cutout on the board not the part. You will get errors but thats is ok. The edge of the board will go through the pad.
2) I can't remember if the "cutout" layer is available in board editor. This will also give the same errors.


Well-Known Member
Found this text written by Richard Hammerl at https://www.element14.com/community/thread/17176/l/custom-pad-shape-creation?displayFullThread=true

The typical way to draw an arbitrary pads shape is:

- Place a PAD or SMD

- Use POLYGON to draw the final pad shape

- For a SMD typically in Layer Top

- For a PAD you have to draw the final shape in all the layers you plan

to use (Top, Bottom, Inner layers...)

The PAD/SMDs center must be inside the polygon's area. Otherwise

that polygon is not recognized as a part to the pad. Use a reasonable

wire width for the polygon, which fulfils the Design Rules.

- The alternative to POLYGON is WIRE

Start the wire in the origin of the PAD/SMD. You have to draw this

area in any signal layer you plan to use. Please use a reasonable wire

width, which fits to the Design Rules.

- Check the solder stop mask

Mask data will be generated for the PAD/SMD area only. Display

layers 29, tStop and 30, bStop. If you want to have the area not

covered by solder stop lacquer, draw it manually in the appropriate


- Check the cream frame (solder paste mask)

Display layers 31, tCream and 32, bCream for this. As we agreed upon

defining packages always on the top side of a board, the layer we have

to check is 31, tCream. Mask data will be generated automatically for

the SMD area only. If this is not what you would like to have, simply

draw the mask manually. Keep in mind that it is possible to switch off

automatic generation of mask data in the SMD properties (Cream



Well-Known Member
Most Helpful Member

That is good. I have done this and it works. I have several ways to do that and one has Design Rules Errors. The boards come out fine but there is an error that must be ignored .

When I first started making "planar transformers" (transformers made from PCB material) this is my first try. It is a part, using 4 layers, vias, through hole pads, and strange cutouts for the core material. The center round leg of the core is shown and the two odd shaped legs are not shown.
This design had too high resistance but did work. The next design was very different.
Just to show you can make a part look like almost anything.
Not open for further replies.

Latest threads

EE World Online Articles