Eagle – Package (Layout Symbol)

Package Footprint

  1. Control Panel>Expand Libraries>Right-click on desired .lbr>Open
  2. Click on Package Icon on top tool bar> type name of package in New box>Ok>Yes

Grid

  1. Type GRI
  2. English units: 0.05″, 0.005 Alternate
  3. Metric: 1mm, 0.1mm Alternate
  4. (Hold down Alt button to use Alternate grid)

Create part outline on Documentation Layer

This outline shows up during board layout, but is not on silkscreen.

  1. Click Wire (Same as Draw Lines) in left-hand tool bar
  2. Click MMB>Select  Layer 51-tDocu
  3. Draw an arbitrary box around origin> Hit escape to stop drawing wire. This final goal is for the outline to fully enclose the package, including pads.
  4. Click Info icon in left-hand tool bar> Click left side of package
  5. Enter wire endpoints on top boxes. Make symmetric around (0,0)
  6. Repeat for right side of package

Add Pads

  1. Change grid from English to Metric if needed
  2. Click Smd or Pad (for through-hole) in left hand toolbar
  3. Enter dimensions in top line “0.4 x 1.5” (without quotes)>Enter
  4. (To change pad size later:  wrench>Smd>…> .2×1.5 )
  5. Left click to place. Keep placing pads until done.
  6. Type “Name” to rename pads> Click on pad 1 and rename to “1”, etc.
  7. To locate pads: Click ‘i’ button, click on pad, enter  x,y, of the exact location of the center of the pad.

Add Pin 1 circle on Silk Layer

  1. Click Circle on left-hand toolbar
  2. Click MMB > Layer21, tPlace
  3. Hold down Alt button to use Alternate grid
  4. Click where the center of the circle should be, then move cursor to define radius

Add outline to Silk Layer

  1. Click on wire, make sure Layer 21 is selected, hold ALT, draw box inside pads.
  2. Change thickness to at least 8 mils or 0.2mm: Click Wrench>Width>…>0.008>Click on lines and Pin 1 circle

Add >Value & >Name

  1. Click Text> Type “>Value” >Select Layer27,  tValues
  2. Click Text> Type “>Name” >Select Layer25,  tNames
  3. Change size: Wrench>Size>…>0.04 (1 mm)   Or enter “cha siz .04)
  4. Change ratio: Wrench>Ratio>13%  Or enter “cha rat 13”
  5. Move “>Name” to best guess as to where reference designator will be
  6. Move “>Value” to somewhere close to package.

Check Solder Mask and Solder Paste layers

  1. Layers > click on 29 tStop. This is what Eagle calls the solder mask layer. Make sure this layer was generated correctly.
  2. Layers > click on 31 tCream. This is what Eagle calls the solder paste layer. Make sure this layer was generated correctly.

Add Description and Save

  1. Click Blue Description at bottom: “This footprint is untested! Used with the FT230X.
  2. File>Save

Leave a Reply

Your email address will not be published. Required fields are marked *