Allegro Board Setup

File--New--
  Board
  Drawing Name: ( name of board )
  ( browse to directory where board will be created )

New PCB ... start here:
Drawing Format
   File Open--ProjectLibrary--TechServices--PCB_Layout
   --Layout_Libraries--Board_Templates
      ( choose appropriate drawing size EG: B size 4 layers )
   Save file in your project: do not write over the TechServices file 

---0---
Existing PCB ... to add a drawing format:
Setup--Design Parameters
  Design Tab
  Extents ( set size of drawing area eg: B )
          ( Left X: -4000  Lower Y: -3000  )
          ( Width: 17000   Height: 11000   )
  Apply--OK
Place--Manually
  Advanced Settings Tab 
    List construction
       Library checkbox
    Symbols and Modules Definitions
       Disable radio button
  Placement List Tab  
    Pull Down "Format symbols"
       Format symbols
         BSIZE checkbox
  Symbol attaches to cursor
  Click in Command: area
    Type in x -4000 -3000
  Done
  Make class visible ( Color Dialog--Drawing Format--All checkboxes
    Apply
Place--Manually
Placement List Tab  
    Pull Down "Format symbols"
       Format symbols
         CLASS_II_FABRICATION_NOTES checkbox
  Symbol attaches to cursor
    Place and click
    Done  
---0---


Setup--Outlines--Board Outline
   w/ dialog box displayed, left click near 0,0, then left click at opposite corner
   Close
   Save

Import Netlist
   File--Import--Logic
      Design entry CIS (Capture)
      Import directory: ... browse to netlist
         ( sub-directory "allegro" )
      Click "Import Cadence"
   
Placing Parts
   Place--Manually
   Click box: Components by refdes
   First part attaches to cursor
   Move cursor to desired location, left click places part
   Next part attaches to cursor
   Repeat
   Click box: OK
   
Moving Parts
   Click the "Move" icon ( four arrow device )
   Click on part to move
   Part attaches to cursor
   Click again to place

   Move to bottom of board: Mirror
   
Rotating Parts
   Click the "Move" icon
   Click on part to move
   Rt Click, select Rotate
   Move cursor around to spin the part
   Click to exit Rotate mode
   Move cursor to position part
   Click to place the part
   
Moving Text
   In the "Find" box, All Off, then click "Text"
   Click the "Move" icon
   Click the text to move
   Rotate w Rt Click
   Click to exit Rotate mode
   Move cursor to position text
   Click to place the text
   
Changing Existing Text Size
   Set visibility, eg: RefDes/Silkscreen Top
   Edit--Change
   Options Tab, set desired Text Block
   Drag a box around text to be changed
   Rt Click "Done"

Editing an Existing Shape
   Shape--Select Shape or Void
   Click the shape
   Use the " drag arrows "
   
Updating a PCB footprint
   After making the change to the footprint in the library
    ( Remove the old padstack from the library ! )
   Place--Update Symbols
   Dialog box, check Package symbols
   Refresh

Set global thermal reliefs
   Setup--Design Parameters--Shapes Tab
   Edit global dynamic shape parameters...
   Radio button Use fixed thermal width of:
     Type in desired width
   Click OK--OK

Via's
It is alwars a good idea to have at least two different kind of vias - smaller vias for signal routing and bigger size via power power and ground signal routing. The bigger vias increase the current carrying capaity but they occupy more space and are potebtially not good for signal integrity purpose. Vias inside the BGA area have to be very small in order to fit in the small space.

Once you have defined two or more different types of vias, you need to assign them to different nets. This is done using the Constraint Editor. The steps involved are

- Go to Constraint Manager ,select Physical, Physical Constraint Setup.
- Select the power nets and double click the cell under via. Assign the bigger size via for the power nets. Repeat it for all the power nets.
- If any signal via need bigger or special via assign it accordingly.

Once you do that, the right vias are automatcally assigned as you route and drop vias. 

Renaming Components and back-annotating
   Make a backup copy of your board before re-naming
      ( there is NO " undo " )
   Logic--Auto-Rename Refdes...
   More... allows setting up details
      Clear the boxes
         Top Layer Identifier:
         Bottom Layer Identifier:
         Skip Character(s):
      Check box: Preserve current prefixes
      Close
   Rename
   This creates a file " rename.log " in the LOG directory
      Edit this file in a text editor
      Remove the header and tail secions (incl white space)
      Remove all the OLD and NEW
      File should be two columns of Refdes
        Old in first column
        New in second column
      Save the file as "was_is_file.txt"
   Open OrCAD CIS design file
      Tools--Backannotate
        Layout tab
      Browse to "was_is_file.txt"
      Click "OK"
   
Save the file