Allegro Footprint Design

Make pads first
  Start--Programs--Cadence--OrCAD 16.x-OrCAD PCB Editor Utilities--Pad Designer
  Drill and symbol first tab
  Layers second tab
    Solder mask 6 mils larger than pad        ( 0.152 mm )
    Thermal relief 10 mils larger than pad    ( 0.254 mm )
    Anti pad 10 mils larger than pad          ( 0.254 mm )
  Name Convention:
    60c35d  60 mil circular pad 35 mil drill  ( 1p52mmcp89d )
    60s35d  60 mil square pad   35 mil drill  ( 1p52mmxp89d )
  Surf mnt ( single layer mode )
    50x75   50 mil x 75 mil y                 ( 1p27mmx1p91 )
    
Package
  Start--Programs--Cadence--OrCAD 16.x--PCB Editor
  File--New--Package symbol
  Drawing Name:_______ Location:________
  Setup--Design Parameters--Design TAB
    Size:
      User Units: Mils
      Accuracy 2 (decimal places)
    Extents
      Left X -2000.00    Lower Y -2000.00
      Width 4000.00      Height 4000.00
    Move origin
     x: 0.00            y: 0.00
    Drawing type
      Package  symbol
 
  Reference Designator
     Layout--Labels--RefDes
     Options--Ref Des--Silkscreen_Top
     EG: J* for a jack, U* for an IC
     ( Text Block 3 is usually OK.  To see all Text Blocks, click the ... button )

  Layout Pins
  Options window: 'pin' it open
  Choose Padstack by clicking on the "..." box
     Padstack attaches to cursor
  Click on Command: 
     x -1000 0     ( places the chosen pin at location x -1000 y 0 )
  Zoom out to see the pin
  Right Click " Done "
  Choose another Padstack
     Padstack attaches to cursor
  Click on Command:
     x -950 100    ( places the chosen pin at location x -950 y 100 )
  
  Editing pin numbers:
     Edit Text ( make sure pin number is visible )

  Silkscreen Outline
     Options--Package Geometry--Silkscreen_Top
     Setup--Grids...
        Non-Etch  Spacing  x:  1
                           y:  1
     Add--Line
        Line width:  10.00     ( 0.25 mm )
        Enter start position in Command:  x -1163 175
        Draw the line w mouse, click at endpoint
        Rt Click--Done
        
  Package Boundary
     Setup--Areas--Package Boundary
        Click to draw polygon
        Rt Click--Done
  
  Package Height
     Setup--Areas--Package Height
        Select package polygon just created
        In Options Box, type in Min and Max heights
        In the drawing window, Rt Click--Done
        
  To change a padstack of an existing pin
     use Tools--Padstack--Replace

  To view drill holes
     Setup--Design Parameters--Display tab--check boxes:
       Display plated holes
       Display non-plated holes
       To set color of drill holes:
         Color Dialog--display--Drill holes:
         Click on a color ( eg: black )
         Then click on Drill holes: " box "
         Apply--OK

  To edit an existing shape 
     Shape--Select Shape or Void
     Click on the shape
     Use the "drag arrows"    

SAVE