Skip to content

Latest commit

 

History

History
145 lines (101 loc) · 7.54 KB

tips.md

File metadata and controls

145 lines (101 loc) · 7.54 KB
Raw

Eagle Tips

Using Eagle

Ubuntu Installation

  • To use 32bit libraries, install the following:
    • For 12.04 or earlier: sudo apt-get install ia32-libs
    • For 13.04 or later: sudo apt-get install lib32z1 lib32ncurses5

Standards for part names (e.g. Resistor → R, Relay → K)

Hide certain airwires:

  • ratsnest ! gnd

Flip text

  • check the spin box when editing the text

Filled in circle

  • set the line width of a circle to 0

Ripup only polygons (useful when running rats and having polygons fill)

  • rip @;

Run ratsnest without having polygons fill at all

  • set polygon_ratsnest off

Delete excess layers (hack stolen from here):

  1. Open the DRC
  2. Go to the 'Layers' Tab
  3. Change the 'Setup' field from "(1*16)" to "1*16" [remove parentheses]
  4. Click Apply
  5. Change the 'Setup' field back to "(1*16)" [seriously]
  6. Click Apply

Making Parts

Symbols

  • Don't change any of the grid / options / etc when making the part symbol. Doing so will make your life miserable.
  • Always add >NAME and >VALUE tags to the board. Make sure that they are on the correct layer, i.e. Names (95) and Values (96) respectively.
  • If multiple pins have the same name (e.g. GND), make sure to add a hint to the corresponding pin (e.g. GND on pin 1 and 2 will become GND@1and GND@2. This will be valuable when connecting symbols and packages when creating the device later-on.
  • Define pin types for pins which are not I/O (the default): you will want to have VCC and GND on the pw option, not connected will be nc and one-directional pins should be defined as in and out respectively. This will help Eagle in detecting wrong connections in the DRC (design rule check) and ERC (electrical rule check) while designing the board.
  • To hide pin numbers in the schematic (as they tend to clutter the overall representation), use the Change→Visible→pin tool on all pins.

Packages

  • Put things on the right layers and use the 'magic strings', that is: >NAME → tNames (25), >VALUE → tValues (27)
  • Make sure you include a part outline
    • You can do this on either tDocu (51, won't appear on final board) or tPlace (21, will appear). Often tPlace is the better choice as having part outlines is nice when assembling boards.
  • Make sure you include an orientation marking:
    • Put this on tPlace (21)
    • Put it somewhere that will not be covered by the part once the part is on the board. It's convenient to be able to glance over a board and verify things are assembled correctly.
  • Many datasheets include a recommended footprint which will give you a good idea for the initial design.
  • To prevent too much solder paste from unevenly spreading across the exposed GND pad below the chip, it is useful to create the inner SMD zone with the option Cream unticked (using Info after creating it). You can then manually add rectangles on the tCream layer (31) and only cover parts of the pad with paste.

Devices

  • Make sure to add a useful description to your device. You can also include links, e.g. to the manufacturer's website, directly using HTML: <a href='www.lab11.eecs.berkeley.edu'>Great source!</a>.
  • Add a "Prefix" to your part (See above for standard part names)
    • The Prefix button is in the bottom right of the window
  • Add an "Attribute" that has the vendor / part number
    • The Attributes "button" is in the Description section to the left of the packaging specifics; it looks more like a URL than a button.
    • When you add a "New" attribute, set its Name to a vendor (e.g. DIGIKEY) and its Value to the vendor part number.
    • Useful Attributes are:
      • DATASHEET (link)
      • DESCRIPTION (string from Digikey)
      • DIGIKEY
      • MOUSER
      • MANUFACTURER
      • MPN (Manufacturer Part Number)
  • Change the symbol name (usually G$1$) to something nicer-looking, e.g. U1, using the name tool.

Board design

From the beginning, you should consider whether you will be hand-assembling parts or use machines. For hand assembly, only use passives with a package of 0402 or larger (no 0201 if possible).

Schematic

Some tips to be followed:

  • People tend to read circuits left to right and top to bottom; try to keep anything with labels or other text oriented that way.
  • Use flag labels only as terminators; standard ones are more readable when labeling a wire, especially printed.
  • If you use flag labels, don't use them for signals which are also connected by wires. Either you use flags for all instances of the signals, or you draw wires. Connecting parts with wires implies that it is the only connection; a mixture with flags will cause you to forget about some references and will make the schematic less readable.
  • Add Descriptions to your schematic sheets (Right click→Description)
  • Add tolerance values directly in the value of passives (e.g. 1k 1%) so you'll remember them when creating the BOM.
  • Make sure to add enough debugging options (test pads, debug headers, FTDI) so that you can test all buses (SPI, I2C).
  • Add enough ground pins (logic analyser, oscilloscope, serial for debugging) for debugging.

PCB layout

Some tips to be followed:

  • Leave enough space between parts, especially around ICs. We recommend at least 12mils on space-constraint boards between caps, and 20mils between caps and ICs.
  • Try to keep all components on the same side of the board; it will make your life easier during assembly as you can only heat up one side with the hot plate.
  • Dont put labels on vias; they tend to become unreadable (overlapping traces is fine).
  • Keep traces to crystals short and straight (they are RF traces due to their MHz frequency!). Decaps for the crystals must not be in-between crystals and pins.
  • Label all testpoints; it is annoying having to open EAGLE every time you want to test something, and other people might not have that possibility.
  • Exclusively use vector font.
  • To create the silk screen: Only enable tNames (25), then group all the names, use the Reposition attributes and apply it to the group by right-clicking onto Reposition: Group. Do the same thing with the Change tool and use Size: 20, Ratio: 18 as well as Font: vector.
  • Make the ground pour polygons have a lesser rank (usually 6) so that your keepouts and similar polygons are not of the same rank.
  • Add version number, date (YYYY-MM-DD) and your name; it will help people to identify who and when somebody designed the board and helps you keep track of different version numbers.
  • Make sure that physical components (such as screw heads) have enough space (it might make sense to draw dimensions in silk).

Check-list

  • How do you power it? Did you consider current and voltage levels?
  • How do you programm it?
  • How do you debug / test it and make sure things are working? Did you add test pads, headers and LEDs?
  • What are you most worried about? (Go read the datasheet again)

Legacy Tips

These help out with older versions of Eagle, but aren't as needed any more

Copy parts from one sheet to another:

(As of Eagle 8.1.1 you can just ctrl-c / ctrl-v! Crazy!)

  1. copy the part
  2. select the part with the group tool
  3. use the move tool, right click and move group, and then move it to the other sheet