What is EAGLE?
CadSoft EAGLE is an app for designing printed circuit boards. EAGLE is an acronym for "Easily Applicable Graphical Layout Editor." It has tools for creating circuit schematics and for laying out the physical wiring and component placement of circuit boards. The software can read EAGLE board files (with .brd extension) and cut them on the milling machine with almost no configuration or setup on the user’s part.
Where do I get EAGLE?
You can download EAGLE from the site.
When you install EAGLE, you have the option of using it for free, with some limitations. The free version is all you need in order to make boards with the milling machine.
How do I import an EAGLE file to the software?
There are two ways:
- With the software open, drag your .brd file into the software window.
- In the software, click the Import Files button and select your .brd file.
If I’m using EAGLE to design boards for the milling machine, what should I know?
- You need to have enough space between the components on your board that the milling machine’s tool can cut between them. For example, if you’ll be using a 1/32" end mill, your traces, pads, vias, etc. need to be larger than 0.03125" apart. You can use smaller tools, like a 1/64" end mill, which allows you to place objects closer together. For more details, read the PCB Design Considerations guide.
- If you’ll be using surface-mount (SMD) components, the pads need to have enough space between them for the tool to fit. Check the Surface-Mount Package Compatibility guide to make sure. If your package isn’t listed, you can test if it'll work by making an EAGLE board file, importing it to the software, and looking to see if there are cut lines between the pads.
- If your board has vias (electrical connections between the front and back of the board), you'll need to create a connection between them. The simplest way is to put a piece of wire in the via hole and solder both ends, but you can also use via eyelets (aka rivets), which sit neatly in the holes as you solder them. You can also use tinned wire, which you can thread through all the holes much more quickly than eyelets or individual bits of wire.
- The holes for pads and vias need to be large enough that your tool can drill them. If you’ll be using eyelets, your holes also need to be large enough for the eyelets to fit. The software will render what it thinks the machine can cut. If it looks like something’s been left out, add a smaller tool or change element sizes.
- You can have the autorouter avoid certain areas and not use through-hole pins on components as vias. This is handy when you're using components that can’t be soldered easily on both sides of the board, like pin headers. Place polygons in the tRestrict (41), bRestrict (42), and vRestrict (43) layers to protect around the places you don’t want the autorouter to put traces or place vias for the top and bottom of your board.
- Slotted/oval holes (the G85 command) are not supported. If you need a slot, make a row of overlapping holes that are a few thousandths of an inch larger than the tool and overlapping by about half their diameter. For example, for a 1/32" (0.031") tool, make a row of 0.033" holes, with centers spaced 0.016" apart.
- If you’re using EAGLE 7.2.0 or later and you want to generate Gerber files, you need to choose the Excellon_24 output device instead of the Excellon output device used in previous versions.
Is there a DRC file I can use to make things easier?
Yes! One for each of the main PCB milling tools. You can download the zip file below. If you’ve never used DRC files, they help you find layout-related problems with your board, such as components or traces being too close together. The only issue is that they often generate a lot of errors that aren’t important. When using our DRC files, you can safely ignore Stop Mask errors. The errors you want to look for are Clearance errors, which indicate that the given tool won’t be able to fit between two objects.
Download the EAGLE DRC file.
Is there a CAM job I can use if I want to export Gerber files?
Yes! It exports using the Protel family of file extensions (.gtl, .gbl, .gko, .txt). For more information, see our Gerber files guide.
Download the EAGLE CAM job.
What are some resources if I want to learn more?
My through-holes and vias didn’t cut! What’s wrong?
Try adding a smaller tool to your imported plan file. The holes in your board might be too small to accommodate the tool you've selected.
For example, if you've chosen a 1/32" end mill, but the holes and some traces aren’t rendered with toolpaths, you might try adding a 1/64" end mill. If the holes render, the machine will cut them. If not, you might need to get a smaller tool or go back into EAGLE and adjust drill sizes. Luckily, as you save your .brd, the refresh button in the software's imported plan file window will allow you to update the file with out re-importing it.
When I try to import my EAGLE .brd file, the software gives an error that says “File Import Failed. The file is missing board outline data in the Dimension layer (layer 20).”
The .brd file is missing the dimension layer, which tells the software the shape and size of your board’s outline. In EAGLE, you need to draw a closed shape around your circuits using the Wire tool, and it needs to be on Layer 20, which is the Dimension layer.
When I try to import my EAGLE .brd file, the software gives an error that says “File Import Failed. The file has no traces in the Top layer (layer 1), and no pads or vias (layers 17 & 18), so there is nothing to cut.”
The software is assuming something is wrong with your board because it’s a circuit board with no circuits. If you actually want a board that’s just an outline, you can get around this error by drawing a trace anywhere, then turning off traces and holes after you import your .brd file.
Although we aim to support .brd files as thoroughly as possible, a few known issues do exist in the software’s EAGLE importer. If you encounter one of these issues, please contact us at firstname.lastname@example.org and we'll do our best to assist.
- Thermals don’t always match behavior in EAGLE, particularly when the thermal is intersected in the middle by other elements.
- Thermal widths may not be correct.
- Signal class clearance rules aren’t always correct.
- Polygon “Orphans” flag is ignored.
- Polygon “Hatched” fill mode is treated as solid.
- Polygon “Cutout” fill mode is treated as solid.
- Dimension elements are ignored.
- Text elements are ignored.
Board Outlines in Eagle 8.3.2
In this version of EAGLE, when you switch from Schematic to Board view for the first time, EAGLE automatically creates a large dimensional rectangle on layer 20. This large rectangle is viewed in our software as the board's outline shape, and the milling machine will cut through the full material thickness in this shape.
That workS fine if you actually want this to be the outside shape of your board. However, if you create your own board outline shape on layer 20, then it's important to delete the one that EAGLE automatically created.
If you don't delete the board outline that EAGLE automatically created, then our software will see that there are two competing board outlines and not read the .brd file correctly.
In this example, the smaller board outline sits within the larger automatically created board outline.
If the larger outline isn't deleted, then our software will read the inner outline as a hole and not see the traces.
If the larger outline is deleted, then our software will read the correctly. The intended board outline will be cut, and the traces will be recognized.