- Control Panel>Expand Libraries>Right-click on desired .lbr>Open
- Click on Package Icon on top tool bar> type name of package in New box>Ok>Yes
- Type GRI
- English units: 0.05″, 0.005 Alternate
- Metric: 1mm, 0.1mm Alternate
- (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.
- Click Wire (Same as Draw Lines) in left-hand tool bar
- Click MMB>Select Layer 51-tDocu
- 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.
- Click Info icon in left-hand tool bar> Click left side of package
- Enter wire endpoints on top boxes. Make symmetric around (0,0)
- Repeat for right side of package
- Change grid from English to Metric if needed
- Click Smd or Pad (for through-hole) in left hand toolbar
- Enter dimensions in top line “0.4 x 1.5” (without quotes)>Enter
- (To change pad size later: wrench>Smd>…> .2×1.5 )
- Left click to place. Keep placing pads until done.
- Type “Name” to rename pads> Click on pad 1 and rename to “1”, etc.
- 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
- Click Circle on left-hand toolbar
- Click MMB > Layer21, tPlace
- Hold down Alt button to use Alternate grid
- Click where the center of the circle should be, then move cursor to define radius
Add outline to Silk Layer
- Click on wire, make sure Layer 21 is selected, hold ALT, draw box inside pads.
- 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
- Click Text> Type “>Value” >Select Layer27, tValues
- Click Text> Type “>Name” >Select Layer25, tNames
- Change size: Wrench>Size>…>0.04 (1 mm) Or enter “cha siz .04)
- Change ratio: Wrench>Ratio>13% Or enter “cha rat 13”
- Move “>Name” to best guess as to where reference designator will be
- Move “>Value” to somewhere close to package.
Check Solder Mask and Solder Paste layers
- Layers > click on 29 tStop. This is what Eagle calls the solder mask layer. Make sure this layer was generated correctly.
- 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
- Click Blue Description at bottom: “This footprint is untested! Used with the FT230X.