Getting started with Eagle CAD, schematic capture

This article details how to draw schematics in Eagle CAD, aimed at new users. It will show you how to set-up the design, find the components and create a nicely drawn schematic.

The official Eagle tutorial, included with the software is worth reading. It is located in C:\Program Files\Eagle <ver>\doc and is called tutorial_en.pdf. This article provides additional hints and tips on using the software for common tasks and answeres some frequently asked questions from newcomers.

For tips on making your own PCBs from Eagle CAD, please read my article here

Step 1 creating a new design

Once you open Eagle CAd you will be presented with a screen like this showing the projects:

On my system, I have created an 'Ians_projects' folder, located outside of the Eagle CAD installation directory, this is to make backing up of the files easier. To create a custom project directory, create a new folder on the PC using Windows explorer, then from within Eagle, select Options-> Directories and you will see the following dialogue box:

You can see my custom project folder on drive F:

Going back to the projects folder, create a new project by selecting the project folder and clicking with the right mouse button, select New Project from the menu.

Then select your new project, double click it and then using the right mouse button, create a new schematic:

This opens up a fresh schematic window
I would now save the schematic, giving it an appropriate name.

Part 2 Adding components to the schematic

The first item to add is a schematic border, to do this, click the Add button, of which there are two, one is a text button the other has a symbol, both are shown here:

I prefer to use the textual 'add' button as I can never remember which symbol is the add button.

You will now be presented with a library browser, in the search windows, type Frame you will be presented with the following results:

I tend to use either the DINA3_L or DINA4_L borders, (note L= landscape, P=Portrait), if you are in the USA or Canada, you may want to use the LETTER_L
Note : even if you only have an A4/Letter printer you can still use the A3 or Frame_C paper sizes, Eagle will scale your drawing to fit the printer page.
 Once you click done, you will need to place this symbol. It always place the border so that the origin is in the bottom left of the schematic as shown here:

 This helps to centre everything on the page and looks neater, in my opinion.

Finding the components you require in Eagle CAD can be tricky at first, the Add tool allows you to search for components and you can use wildcards so *741* will return every TTL device with 741 but further down the listing you will find the ubiquitous ua741 op-amp you wanted.

A search facility is good but what if you want to browse or do not know how to specify say a 0.5W metal fim resistor or 100uF through hole capacitor? The next section will help

Part 3 finding common components in the library

With the standard installation, Eagle comes with a wide variety of libraries, with more available from Cadsoft and other sources on the internet, which is fine but for commonly used parts, how do you locate them?

Starting with the passive parts first. From a schematic, click the 'Add' button and scroll down to the RCL library and expand it out.

As I am based in Europe, I use the European (EU) symbols for resistors, capacitors and inductors. If you prefer the US symbols, select them instead.
For any of the libraries, expand the library and you will see a list of components. Use the following table to help find the part you require, note SMT = Surface MounT, PTH = Plated Through Hole.

Component	Range of values	Library	Name	Description
Ceramic Capacitor (PTH)	10pF to 1nF	C-EU	C025-025X050	2.5 mm pitch, 5 mm outline
Ceramic Capacitor (PTH)	1nF to 220nF	C-EU	C050-030X075	5mm pitch, outline 3x7.5 mm
Ceramic Capacitor (SMT)	10pF to 100nF	C-EU	C0603	Typical range for 0603 size,check your specific part
Caermic Capacitor (SMT)	100nF to 47uF	C-EU	C1206	Typical range for 1206 size,check your specific part
Electrolytic Capacitor (PTH)	1uF to 47uF	CPOL-EU	CPOL-EUE2-5	Typical for 10-35V parts. 2 mm pitch, 5 mm diameter.
Electrolytic Capacitor (PTH)	47uF to 100uF	CPOL-EU	CPOL-EUE2,5-7	Typical for 10-35V parts.2.5mm pitch, 7 mm diameter.
Electrolytic Capacitor (PTH)	100uF to 220uF	CPOL-EU	CPOL-EUE3,5-8	Typical for 10-35V parts.  3.5 mm pitch, 8mm diameter
Electrolytic Capacitor (PTH)	470uF to 1000uF	CPOL-EU	CPOL-EUE5-13	Typical for 10-35V parts, 5 mm pitch, 13 mm diameter.
Inductor (PTH)
Inductor (PTH)
Inductor (PTH)
1/8W resistor (PTH)	Various	R-EU	0204/5	5 mm grid
1/4 to 1/2W Resistor (PTH)	Various	R-EU	0207/7	7.5 mm grid
1 W resistor (PTH)	Various	R-EU	0414/15	15 mm grid
3 W resistor (PTH)	Various	R-EU	0617/17	17 mm grid
1/16 W resistor (SMT)	Various	R-EU	R0603	Typical power for 0603 size
1/4 W resistor (SMT)	Various	R-EU	R1206	Typical power of 1206 size
1 W resistor (SMT)	Various	R-EU	R2512	Typical power for 2512 size

The values and types listed above are typical based on component data taken from manufacturers data. Always check the sizes for your particular parts to ensure they are the correct size.

Commonly required parts and their location

Component	Library	Notes
Pin strip header	Pinhead	0.1"/2.54mm pin header
Drill holes	Holes	Select drill hole or mounting pad and size required
USB connector	CON-USB or CON-USB2	Select required types, double check footprints.
Crystal or oscillator	Crystal	Check footprints
Power connections	Supply	More on this later
Toggle switch	Switch	Numerous switches
Test pad/solder pad	Testpad	Choose the pad to meet your requirements.
SUB-D/D-type connector	con-subd
Transformer	trafo or inductor-neosid
Screw terminal connectors	con-wago, con-wago500 or con-wago508	Screw block terminal, 2.54 and 5mm pitch
DC power plugs	con-jack	Used for mains adapters

Finding other components
For the following component types, it is easier to use the search function:
Op-amps
Logic gates
Power converters e.g. 78*05
Diodes
LEDs
Memory devices
Microcontrollers
anything not covered previously

Step 4 drawing the schematic

Hopefully by now you have set-up a new drawing, found the parts you require and placed some parts on the schematic. This section will not teach you how to draw a schematic but it will provide hints on common queries

Adding power pins and logic gates

As an example, your design uses a 74AC04D hex inverter, and you have used 5 gates, how do you load the 6th unused gate, to tie it's input to ground. Use the 'Invoke' button:

Next click the device, IC1 and you will be presented with this menu:

Click on 'Gate' F to load the unused device and click OK, the invoke tool should still be selected so click on IC1 again and select 'Gate' P to load the power pins, then click 'OK'. You have now placed the power pins.

It is easy to forget this step when using TTL logic devices but with any complex part that does not show power pins, be sure to try the 'Invoke' command.

Adding power nets

Related to the previous section, you will want to add power nets to your design. To do this, use the 'Add' command and navigate to the 'Supply' library, from here you can add a Gnd net and various positive and negative power supply nets.

Check your design

Always check your design, use the design rule check option, either click the DRC icon or use the Tool-> DRC menu item. This will save you some hassle later on.
On my simple example design, with no connections the following errors were flagged up:

Whilst this is to be expected it does highlight the fact that the software checks for unconnected inputs and missing power supplies, very important checks for any design. It will also warn if nets are shorted together.

Updated 05 May 2012