The purposes of these folders are to store the different parts of eagle. Over time you will need to make your own parts and components, and use more libraries than comes with the eagle by default. These library files go to this directory you set for the libraries.

Design blocks

Design blocks are functional circuits you have designed and specially saved as design blocks. They are not the whole board, but they are the usage of different components. You will run into different components that have their minimal recommended components for them to work. It will be impossible to remember these components every time, so once you have the elements you need, for say a ATtiny841 chip, you save the chip as a design block, and then just add it as one to anything you need it with.

Design rules

Design rules are a set of guidelines for eagle, that dictate how much room should be left between the traces, pads, holes and components. It is a good idea ot use 0.4mm or 16mil for these values, but in the end the proper values depend most on the machine and the bits you have for it. Chances are your lab has its own preferred desing rule file.

Projects

Projects, this is the folder where all your work goes, all the schematics and boards you make

the reason I have changed the directories is, that I have moved them to a clouddrive, letting me access all my work even on the go. Also, because as autodesk pushes out new updates to eagle, and they are right now quite prolific at it, the contents of the default directories dont get copied along. Still the new version of eagle automatically reads the folders listed here, so you are good to go as soon as the install is over.

To add individual components, you need to open the add menu and find the component you wish to use. Initially this can be daunting, because there are so many of them. Which is the right one? In this case we we used the component library that has most of the fab lab inventory components, but it doesnt have all of them but it is a good starting point for most projects at the lab. Over time you can make your own libraries that have the components you prefer to use.

Through repeating this again and again for each of the different components you need, you can then add all of the components you need. when you have chosen a single component, you can put more of them just by clicking again and again, to return to the component adding window you just need to press ESC, and you can then either pick an another component or close the window by pressing cancel.

Here I have added all the minimal components for the ATtiny841 chip, I gave it a clock, couple capacitors to keep its power nice and neat, and the ISP programming interface. While the clock is not critical for its function, I like to have the option for it on my board. This is my default design block for this chip.

After adding your components you need to wire them, in my image they are the green lines between the components, called networks. Next to the net icon, is a similar but a blue line, it is for making a BUS. It is a logical tool for keeping networks together, you define the networks that will travel in the bus, by naming the bus after them separating the different nets with a comma. So far I have not had to use the bus at any point for the fab academy assignments.

But something looks wrong initially doesnt it? why the clock and IPS header are not connected like the components between vcc and gnd or the components for RST? If everything was connected with the network lines directly it would look like spaghetti that would be hard to understand. So Instead we name the networks, the naming then connects them logically. So that the clock is connected to two networks, the XTAL1 and XTAL2, and those networks are connected at the specific pins on the chip, forming the connection of the clock to the chip.

Now that we have all the components we need connected, its time to design the board itself. This is a good deal trickier, you need to make the board file, the software makes it automatically when you just try to switch to it the first time.

Then you get the ratsnest, that is initially a real mess. The more components you have, greater the mess it is. The yellow lines are called airwires, and are eagles way of complaining that it doesnt see a connection between parts.

You then use the basic move tool to move the components around to place them on the board properly. When you zoom in you can see the name of the network that pad is connected to. But now the airwires are a mess, and makes things confusing. So if you click the ratsnest icon, the program will recalculate the airwires.

Things look much clearer now dont they? so lets connect the pads with the route tool. But before I do that I like to make a little settings change, to the grid we are working on. I like to use the 0.1mm grid, this gives me greater accuracy in drawing lines.

At this point it is also good to sort out the design rules, open the window for them from the side icons. Then by clicking load you can open the directory for them you defined earlier, and pick the design rules file that is for the mill used at your lab. In general you dont need to worry about any of the other tabs, Clearance is the one we want to work with. This defines the distances allowed between the traces and the components.

Then you just click apply, and select. If you set the design rules as one of the first things when making a board, the program automatically enforces them from the beginning.

The thing that makes this part tricky, is that the different networks cant come in contact with eachother directly. But one helping feature is that you can pull traces under components, if you need to pull a trace over an another you can use a 0ohm resistor to pull it over the other trace. When you get good enough to make double sided boards, you can drop the trace to the other side instead of using 0ohm resistors.

Also some other components can be used for pulling a signal over others, with my DRC I can pull 4 lines under the omron buttons our lab uses.

But why havent I connected the GND? Ss you can see all other traces are done, but the ground is not connected. It is possible to connect the ground just like all other pads, but it is not the only way. I like to use the ground plane. To make it I have to draw a polygon, by pulling a polygon line around the components.

Then that polygon is named GND, to tell the program it is the groundplane. By pressing the ratsnest again, the program "pours" the plane. Now you have something that actually looks like a proper circuitboard.

The plane I named GND can be named to be part of other networks like VCC or any of the networks you made. But in general there is no real need to use it for other than the ground.

If you save the design you made as a design block at this point, you will have both the schematic and the properly wired board ready to be placed into your next project.