Eagle PCB software tips and tricks


  • Hardware Contributor

    I just got my first large (for me) PCB order in and so I've spent a lot of time using the Eagle PCB design software over the last few months. I realize that many/most people are using KiCad since it's open source but I found Eagle first and did a lot of work in it before I saw KiCad so that's what I've stuck with. I thought it might be a nice idea to capture what I've learned about using Eagle effectively and see if anyone else had any tips to share.

    Project names

    Put a version number in the project name. I usually start with v1...vN as I'm iterating designs. Any time you start reworking something (routing, layouts, etc), save it to a new iteration. When you submit an order, move all the extra versions to a backup folder and rename the version you submitted to v1.0 and never change it again. If you need to edit something, create a v1.1 and edit that.

    Hot keys

    To get the maximum efficiency, use hot keys for everything. It's much faster selecting tools and toggling layers if you have keys set up instead of using the mouse. The most important set to me are the display keys (see F9-F12). They allow me to quickly toggle top and bottom layers and toggle polygon filling. It's annoying to set them up because you have to do it in the schematic editor and the board editor but it's worth it.

    The most useful ones are:

    • F9 shows both layers
    • alt-F9 shows just unrouted air wires
    • F10 shows just the top layer
    • F11 shows just the bottom layer
    • F12 fills polygons (ground planes)
    • alt-F12 unfills polygons

    Here are my keys:

    Key Action
    alt-b move
    alt-c copy
    alt-d delete
    alt-e net
    alt-f move
    alt-g group
    alt-i info
    alt-j junction
    alt-l label
    alt-m move
    alt-n name
    alt-q ripup
    alt-r rotate
    alt-s smash
    alt-t text
    alt-v via (board), value (schematic)
    alt-w route (board), wire (schematic)
    alt-z ratsnest
    F9 display 1 tname torigin tplace 16 bname borigin bplace pads via unrouted dimension tkeepout bkeepout trestrict brestrict drills holes milling; display 1 16 125
    alt-F9 display none unrouted
    F10 display top tname torigin tplace -bottom -bname -borigin -bplace -bkeepout
    F11 display bottom bname borigin bplace -top -tname -torigin -tplace -tkeepout
    F12 ratsnest
    alt-F12 ripup @;

    Libraries

    Build your own part library with the parts you'll use. That way you can find things faster and you know whether they work or not. Copy parts from eagle, sparkfun, and other online sources. You can find the library I've created for MySensors components at https://github.com/TD22057/Eagle-MySensors

    Grid

    For the schematic view, stick with 0.1 inch spacing since most of the library parts use that for the schematic symbol layouts (and NEVER use the alternate spacing). This insures wires will snap to the correct location and the connections get made. For the board view, metric or Imperial works. Since most of the parts I use have pins on 0.01 inch spacing, I use a grid with the major size 0.025" and the alternate size 0.00625 which seems to work well.

    Ground planes

    Use 0.012 isolation, 0.010 line width. The smaller line width allows the ground plane to flow between pads better. If you ever see a ground plane not going between a pad you think it should - it's probably the line width.

    Silk screen

    0.032, 15% is the smallest text size I would use on a board. That's readable (in good light) - but I usually prefer things to be larger than that. Once your board is done, smash all the parts to separate the text and parts, then position the labels in good locations. Add your own labels with the text command - make sure they're in the tPlace layer - that way the panelize ulp will duplicate them correctly.

    Scripting

    Eagle has a scripting language which I don't really understand. But - if you have any task that seems tedious (changing lots of items, spacing many components on a grid, etc), someone has probably already written a script to do it so search the web for Eagle scripts.

    Design Rule Checking (DRC)

    Obviously you need to run DRC often to make sure you haven't violated any rules. Download the DRC file from your manufacturer and use that. I normally copy and edit that file and make it more conservative and use that for my DRC run. The more conservative you can be, the less likely there are to be errors in the board when it's made.

    Viewing your board

    Use http://3dbrdviewer.cytec.bg/ to upload the board file for 3-d viewing. This can help visuallize how close things are together. In addition, you can download EagleUp and use it to export your board to SketchUp for 3-d viewing. Each part in your board will require a SketchUp object with the same name but they're pretty easy to find. This can really help visuallize how components will fit together.

    Ordering your board

    Before placing an order, run the renumber ULP - that will insure that parts are numbered in a reasonable order (so R12 isn't next to R1). Then adjust all the labels until you're satisfied.

    If you need to "panelize" a board (make duplicates of a single board in a larger board), you can do that. Close the schematic view and save the board to a new file. Run the eagle panelize.ulp - that will copy all the names from the tNames and tPlace names to a new layer. Then do a group, copy on everything and position the copy. Repeat as necessary. The problem with the copy is that each part gets a unique name which makes the labels wrong. But, the copied names in the new layer are correct so when you export the board for manufacture, select that layer instead of tPlace and tNames and the labels will be correct. See this panelize tutorial for more details.

    Be sure to download the CAM job from whatever board house you use (so far I've had great results from Elecrow) and run that to generate the gerber files for them.

    Boards larger than 10cm x 8cm

    The free version of Eagle limits boards to 10cm x 8cm. If you can split your order into smaller pieces (say two 10cm x 5cm or four 5cm x 5cm boards), you can use eagle-brd-merge to merge multiple board files. It takes in an offset and rotation for each board and writes out a new board file with the merged result. You won't be able to edit anything outside the 10x8 cm area but it works great for combining multiple boards into a single panel.



  • Very interesting ! Thanks !
    I will use all these tips very soon !

    David.


  • Admin

    @TD22057

    Instead of the hassle of renaming the project etc. You can use git to version your work. Add a tag to your commit everytime you make an order, and mark your board so you can see what version you got back from the board house.


  • Hardware Contributor

    for grid, I would add grid pitch depends on the board density. If dense, a big pitch is not very doable 😉
    An important ulp : zoom_unrouted.ulp to check if you have airwire.
    so much things to say...

    Nice post 🙂


Log in to reply
 

Suggested Topics

  • 5
  • 1
  • 2
  • 13
  • 10
  • 1
  • 3
  • 6

0
Online

10.3k
Users

10.7k
Topics

109.7k
Posts