Forward annotation to PADS PowerPCB (Lepton EDA Reference Manual 1.9.18)

#### 6.4.1 Forward annotation of lepton schematic changes to PADS PowerPCB layout ¶

#### 6.4.1.1 Overview ¶

Forward annotation is the process of updating a layout to reflect changes made in the schematic. This process is used when, for example, a new component is added to a schematic and needs to be included in the layout. This section describes how to forward annotate changes in a Lepton schematic to a PADS PowerPCB layout.

PADS implements forward annotation through the use of an ECO (Engineering Change Order) file. The ECO file describes the differences between a current design and the desired design. PADS generates the ECO file by performing a netlist comparison between a new netlist file and the netlist contained in the current layout.

#### 6.4.1.2 Detailed forward annotation procedure ¶

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

- Create an updated PADS netlist by running:

  `lepton-netlist -g pads -o mynet.asc pg1.sch pg2.sch`

  This will create the netlist file `mynet.asc`.

- Make a backup copy of your PADS layout in case things fail in a destructive way.
- From within PADS, choose the Tools → 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
√ | generate differences report
√ | generate eco file
comparison options
√ | compare only ECO registered parts
attribute comparison level
√ | ignore all attributes

Click the ‘`OK`’ button to create the ECO file.

- 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).
- From within PADS, choose the File → Import... menu item. Locate and choose the ECO file created previously.