Monthly Archives: December 2013

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

Eagle – Schematic Symbol

Symbol (Schematic)

  1. Control Panel>Expand Libraries>Right-click on desired .lbr>Open
  2. Click on Symbol Icon on top tool bar> type name of symbol in New box>Ok
  3. Enter “grid” in top line. In dialog box: Size: 0.1 inch, Multiple: 1, Alt: 0.01

Draw symbol outline

  1. Click Wire on left-hand menu and draw a box (should be on Layer94)

Add Pins

  1. Click Pin on left-hand menu>Click Short on top menu>Place all pins around package
  2. Right-click to rotate pins for the various package sides. The “circle” should go away from the package.

Name Pins

  1. Type “Name” > Click on each pin and give descriptive name (GPIO5 or !RST). Can put “!” In front of the name to indicate active low. Pin will then have an overline.

Set Pin Direction (io, in, out, pwr)

  1. (Optional) Wrench>Direction>pwr>Click on all power and ground pins, etc.

Move pins around to preferred location on symbol

  1. Type “move”> Move pins to desired location around symbol.
  2. Can also move package outline if needed by clicking on a corner or edge.

Center symbol

  1. Type “group”>Click and drag across entire symbol, release
  2. Ctrl-Right-Click and move until “+” is in center of symbol

Add “>Value” & “>Name”

  1. Click Text> Type “>Value” >Select Layer96,  Values
  2. Move “>Value” to bottom of symbol, just below box
  3. Click Text> Type “>Name” >Select Layer95,  Names
  4. Move “>Name” to top of symbol, just above box
  5. Change size: Wrench>Size>…>0.07> Click on both “>Value” and “>Name”

Add Description and Save

  1. Click Blue Description at bottom: “Schematic Component for FT230X.”
  2. File>Save

Eagle – Device Creation

Device Creation (Tying symbol and package together)

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

Add Schematic symbol to Device

  1. Click “Add” button on left hand menu> Choose symbol>Drop on the “+” in the center of the window.

Add Package to Device

  1. In bottom-center, Click on “New”>Find desired package and double-click
  2. If package is not found, may need to copy from another library. See post on Library.

Add Variant Name

  1. This is optional: Only needed if multiple variants are used with the part.
  2. Right click on name under “Package” in center of window>Rename> Change the single quote( “) to SSOP or whatever the package is.

Associate Pads with Pins

  1. On bottom-right, Click “Connect”
  2. Highlight a Pin name>Double click a Pad name
  3. Click “Ok” when all assignments are made.
  4. Should see a green check next to variant when done

Change Ref Des Prefix

  1. In bottom-center, Click Prefix> Type “U” (no quotes)
  2. (Optional) Type “Name” > Click “+” in center of symbol, change G$1 to U1

Set Up Value

  1. On bottom, click button to set Value to “On”
  2. Click Attributes in lower-left window. Then click New. In the name field, type VALUE. In the Value field, type the text you want to appear on your schematic.

Add Description and Save

  1. Click Blue Description at bottom: “The FT230X is a simple USB to serial converter”
  2. File>Save