Eagle stands for Easily Applicable Graphical Layout Editor

This is based on Version 5.12.0 for Windows, Professional Edition. Surely they have not changed that much, though.

How to copy symbols between libraries…

Unfortunately, there is no way to directly copy a symbol between libraries. You have to create a new symbol in the destination library and then manually copy the components from the old Symbol to the new.

1. Copy the Symbol name & components from the containing library
   1. Open the containing library
   2. Open the Symbol in the editing window
   3. Copy Symbol name to computer’s clipboard (Top menu: Library -> Rename)
   4. Show all layers using command “Display All”
   5. Create a group using all of the components
   6. Perform command “Copy”
   7. Ctrl + Right-click on group
   8. Close library
2. Create copy of Symbol in destination library
   1. Open the library
   2. Create a new Symbol, use name from computer’s clipboard
   3. Perform command “Paste”
   4. Place components at desired location
   5. Save before closing

How to export BOM….

1. Open Schematic Editor
2. Perform command “run bom.ulp”
3. Set “List Type” to “Values”. Will cause all components of the same type will be grouped.
4. Save, view, or copy/paste the file to Notepad.

Capacitor value standards to follow in schematics…

1. Always use microfarads (uF) for capacitor values.
   1. Convert nanofarads (nF) to microfarads (uF): uF = nF/1000
   2. Helps when generating BOM while grouping by value.
2. If there is a decimal point, ALWAYS put a leading zero.
   1. 10uF => 10uF
   2. .1uF => 0.1uF
   3. .22uF => 0.22uF
   4. .022uF => 0.022uF
3. Do not put a space between digits and unit of measurement.
   1. Examples: 10 uF => 10uF

Fast way to change layers in Board Layout…

1. Perform command “change layer”
2. Select desired layer from popup window
3. Click on object to move to that layer
4. Works for groups as well

How to change package of part in schematic…

1. Go to Board Layout
2. At top of menu: Edit -> Change -> Package
3. Click on part
4. Change

How to change xref label to only display name…

If this is not done, sheet number and numerous other things will be displayed after name like:

“name/4.4a”

1. At top of menu: Options -> Set
2. Misc
3. Set “xref label format” to: %F%N

How to renumber parts in Eagle…

1. Perform command “run renumber-sheet.ulp”
2. Use the following settings:
3. Sort X: Ascending
4. Sort Y: Descending
5. Weighting of emphases: Y-direction

Fast way to change trace width in Board Layout…

1. Perform command “change width .4”
2. Click on trace
3. Works for groups as well.

How to move a group by an offset…

1. Create group
2. Perform command: “move (c>0 0) (x y)”
3. For example: “move (c>0 0) (5 -5)”
   1. Moves group 5 up and 5 to the left

ALWAYS turn on vector font upon reinstall…

1. Options -> User Interface..
2. Make sure “Always Vector Font” is checked
3. Make sure “Persistent in this drawing” is checked
4. Ensures that this document will use the vector font even if moved to a new computer.