Auto Rename Reference Designators

FOLDER STRUCTURE:

   ProjectName
      RevA
         SchPcb
		    FileName.DSN      (Schematic)
            allegro
               FileName.brd      (PCB)

FIRST:

   Backup the PCB file and the Schematic file.

   Ensure that no changes have been made to the Schematic since the last netlist was transferred into PCB

PCB: 
 
   Manufacture -- Auto Rename Refdes -- Rename... 

   Use Default Grid ( radio button )
   Rename all components ( check box )

   Setup ( click the button )

   Rename Ref Des Set Up Dialog box:

      Layer:             BOTH
      Starting Layer:    Top Layer
      Component Origin:  Body Center 
  
      Directions for Top Layer:
         First Direction: Horizontal
         Ordering:        Left to Right   then   Downwards

      Directions for Bottom Layer:
         First Direction: Horizontal
         Ordering:        Left to Right   then   Downwards

      RefDes Prefix  *    ( leave the * in this box )

      Clear text boxes for Top Layer Identifier and Bottom Layer Identifier
	  
	  Skip Character(s):  IOQ
	  
	  Renaming Method:   Sequential
	  
      Preserve Current Prefixes  ( Check the box )

      Refdes Digits:   1
	  
	  Grid Based Renaming:  ( leave blanks )

    Close "Rename Ref Des Set Up " dialog box

   Rename ( click the button )

   Close "Rename RefDes" box

   Verify that the RefDes's were changed as requested

   Export -- Back Annotation Netlist...

   Design Entry CIS ( set the radio button )

   Export to Directory:   .    ( put a . in the text box )

   Export ( click the button )

   Close the "Export Logic" box ( click the X )

   File ... Save
   
CAPTURE:

   Open FileName.DSN

   Focus on Design Resources FileName.DSN

   Tools -- Backannotate...
   Dialog box:
      PCB Editor Tab
      Generate Feedback Files ( check box )

   PCB Editor Board File:  path\FileName.brd

   Netlist Directory:   .  	( put a . in the text box )

   Output File:         .\FileName.swp

   Back Annotation:

      Update Schematic  ( put a check in the box )

      OK    ( click on the button )

   The schematic RefDes's are updated

  Cross probe between the Schematic and the PCB to verify that it worked correctly

  File ... Save