Cadsoft Eagle tips and tricks

From DP

Jump to: navigation , search

Tips

  • If you hold down the Ctrl when you do a move it will snap to the grid.
  • Holding ALT snaps to the alt grid. Hold down alt for small movements.
  • To do a fill, use the "Draw","Polygon" and create a shape. Then right click on it and name it ie. GND.
  • To copy a symbol or package to another, use the "Edit","Group" and drag a box around the object. Click "Edit","Cut" then click on the "Go" traffic sign. Goto the new page and click "Edit","Paste" to place the object.
  • When making a new symbol, to place a bar over a signal name use the "!" character and a bar will be placed over the following characters. (ie. !EN) To terminate a bar in the middle of a signal name use another "!". (ie. !WR!/RD)
  • When making a new symbol, if you have more than one signal with the same name ie. GND, use the "@" character after the name and a number. (ie. GND@1, GND@2) You can use the pin number. Only the signal name will be displayed and not the "@" and following characters.
    • It is ! or ~ or $ or ^ it depends what program you use
    • You can also do that with signals. For example you have a wire CS that is negative true you can name it !CS and the name on the signal/wire will have a bar over it.
  • When making symbols or packages, it is sometimes easier to throw down the pins and outline and use the "Properties" to set the positions.
  • When make new packages, place one pad and then use the "Properties" to set the dimensions. Then "Copy" in order to the other pins.
    • You can type the dimensions into the pulldownbox. i.e. 1.2 x 3.5 The parser is pretty much smart in understanding what you type. The same 'trick' can be used for linethickness, fontsizes, etc.
  • Always do the schematic and symbols in Imperial units because most libraries are in Imperial units. Do the board and packages in either Imperial or Metric.
  • To create a filled circle, set the width to zero. Useful to create a circular keepout area.
  • PCB dimensions are set on the dimension layer (?) with a zero width line too.
  • If you need to make change to a large area then you can select everything and move or rotate, etc. You can also Lock the parts that you don't want to move or otherwise be edited.
  • Look around in the existing library as much as possible, including the free 3rd party libraries. If you see anything at all in them that you don't know how to create yourself, then dig deep and figure out how it works. That how I learned about the ! trick, 0-width circle, @# technique, and basically everything else.
  • If you want to generate some plotting code it should be very simple as you just need to translate the codes 1:1 from gerber to whatever code you need (hpgl, g-code or something else)... but you should check few gerber viewers if they have ability to plot directly
  • Look around in the existing library as much as possible, including the free 3rd party libraries. If you see anything at all in them that you don't know how to create yourself, then dig deep and figure out how it works. That how I learned about the ! trick, 0-width circle, @# technique, and basically everything else.
  • Run ERC and DRC. They are your friends. You can safely ignore anything you've done "on purpose" by clicking on the right button, and Eagle will remember until you move or replace the part.
  • There is also a zoomunrouted.ulp that zooms in on any place that is unconnected. It is a standard part of our PCB pre-flight.
  • If you are trying to create an area without traces or pours, you can create a shapes on the tRestrict and/or bRestrict layers. This is often done in the package drawing to keep traces from going under a particular location under the package.
  • The tKeepout and bKeepout layers will generate errors but will still route through the area.
    • Keepout is designed to allow you to control spacing between parts, that's why routing is still allowed.
    • If you need to leave room at each end of a header for those cables that have really wide connectors, tKeepout will stop you from putting parts in that area (although I'll often sneak a part that isn't tall, like an SMD bypass cap, into that area and 'ignore' the warning).
    • You could make a 'connector' for the Microchip PICkit 2 programmer that has a tKeepout large enough for the programmer to be attached without bumping into anything. You'll get a warning if you place anything too close. If only this feature were 3D!
  • When doing a pour you are sometimes left with some areas that dont pour on one side. Drop a via in that area and name it to the pour on the other side. The area will be filled in with the pour.
  • ALWAYS check the pin numbers. Also, don't forget about potential mirroring if you're mounting on the bottom or planning on soldering a header from the reverse side.
  • Eagle lite will open a multipage schematic. Of course it will only let you edit the first page.
  • To get 'Names' to appear on nets, right click on the net. In the popup menu click on label. Position the label where you want it and left click on the position.
  • Eagle installs a bunch of libraries on its own, and then you can install your own libraries, too.

FAQ

  • How do you change the default dimension unit?
  • How do you change the "Frame" after it has been placed in a schematic?
  • Is it possible (ie. is an add-on available) to "plot" (not to print) a result?
  • Why all libraries do not show up sometimes when using the 'Add' function in a schematic.