Waag Society Fablab Amsterdam

If you have not done so yet, start by creating a schematic in Eagle and come back to this part when you're done. To get started making a schematic please refer to http://fablab.waag.org/project/stereo-amplifier/documentation/5613.

Make sure you have your schematic opened in Eagle, then follow through the following steps to design your PCB.

1. Create a PCB
From the menu select File>Switch to board. Because there is no board yet, Eagle will offer to create one for you from the schematic. Select "Yes" when prompted. You'll end up with something like this:

 As you can see it's a bit of a mess. All the components from your schematic are placed outside the working area of the PCB. The yellow lines are the connections drawn in the schematic. I found it's pretty useful to arrange these components pretty much like the schematic and then continue to the next step.

2. Ratsnest
After moving the components to their positions on the board things don't exactly look prettier.

To remove much of the clutter we'll let Eagle redraw the connections in a more efficient way. To do this we'll use the "Ratsnest" tool from the toolbar on the left. This will leave us with something slightly more agreeable like this:

3. Load Design Rules
In order to make sure the PCB we're designing can actually be made on the milling machine it will have require a certain spacing between paths and pads, the milling bit will have to fit inbetween. First download and save fablab.dru, a set of rules created by Marc Boon. To load these rules we'll have to click the Drc tool. Then press the "Load..." button and load the fablab.dru rules. Once loaded press the "Check" button. No messages should appear, although if you use very small components there might be clearance errors.

4. Create the traces
This is where the magic happens! Press the "Auto" tool, set the top to "N/A", set Routing grid to 5 and press OK. If all your yellow lines have disappeared and turned into thick blue traces your PCB is complete. It's not very pretty and probably way too large at this point, but it's functional.

5. Rip up the traces, move components and recreate traces.
Now you have some idea where all the traces go and where space can be saved break down all your traces by using the "Group" tool. Drag a recangle around everyting on the board, then select the "Ripup" tool, right-click on one of the traces and select "Ripup Group". Alternatively you can use the Edit>Undo function in the menu to undo the creation of the traces.

Now move your components closer together, rotate them as you see fit to get a nice and compact layout. Then move the edges of the PCB inward to fit snugly around your components. Then recreate the traces.

Keep ripping up and moving the components till you're satisfied with the result.

As it turns out I was using the wrong size and capacity capacitors. So I went back to the schematic and fixed that. Also, because these capacitors are quit big I had a lot of spare room on the PCB. In the PCB design screen I went into DRC>Sizes and changed the size of the traces to 3mm.

Eventually I ended up with this:

6. Adding a ground plane
After I was satisfied with the design, I've made the board slightly larger again by moving the edges of the board outward. Then I moved the whole set of components and traces to sit nicely in the middle of the PCB.

In order to create a ground plane first you'll have to draw a polygon around the edges of your PCB. Do this by using the polygon tool. The end result will look something like this:

Then go into the menu and select Edit>Name, then click the polygon you just created, a popup will appear, then rename it to GND. Then you'll get another popup asking you to confirm it can connect this polygon to the GND net. The software will now create a ground plane for you. Mine ended up looking like this:

7. Export PNG files

In order to mill this virtual PCB into a very real one you'll have to export it to .PNG format.

First we'll create a bit of a working area. Select the rectangle tool, then in the drop-down list at the top of the screen select a layer you're not likely to use, I selected 51 tDocu, then draw a rectangle slightly larger then your PCB. I took about a centimeter on all sides.

Because only the traces and pads are needed we'll hide the rest for now. To do so click the "Display" tool from the menu. The easiest way is to click the None button and then switch on the layers "Bottom" and "Pads". Click the numbers before these layers to turn them back on. Then press "OK".

Now click File>Export...>Image. Select a location to save your PCB, name it something like rectifier_traces.png, switch on "Monochrome", change the resolution to 500 dpi and make sure the Area is set to "Full". Then click "OK". This image will be used to mill the traces on your circuitboard.

Then go back into the "Display" settings, click "None" and enable "Pads" and "Dimension". Export this file as rectifier_outline.png with the same settings as before.

8. Editing the outline

The files needed to create your PCB are almost done, and you can now close Eagle. Open the rectifier_outline.png with MS Paint or GIMP. Select the Fill tool and paint the area inside the outline white. The results of both images can be seen below.

Your PCB is now ready for the next step, creating milling and paths.