Detailed Forward Annotation Procedure

This procedure assumes you have a board layout open in Pads and that you have made your schematic changes in gschem. For the purposes of illustration, assume your schematic is split into two pages in the files pg1.sch and pg2.sch.

1. Create an updated Pads netlist by running ``gnetlist -g pads -o mynet.asc pg1.sch pg2.sch''. This will create the netlist file ``mynet.asc''.

2. Make a backup copy of your Pads layout in case things fail in a destructive way.

3. From within Pads, choose the ``Tools$\rightarrow$Compare Netlist'' menu item and choose the following options in the form.
   
   

   original design to compare:	use current PCB design
   new design with changes:	mynet.asc
   $\surd$	generate differences report
   $\surd$	generate eco file
   comparison options
   $\surd$	compare only ECO registered parts
   attribute comparison level
   $\surd$	ignore all attributes

   
   Click the OK button to create the ECO file.

4. Examine the ECO file to make sure it looks ok (the ECO file is a text file which can be viewed with any text editor).

5. From within Pads, choose the ``File$\rightarrow$Import...'' menu item. Locate and choose the ECO file created previously.