Importing a netlist into PCB123

[Sal Hernandez]

PCB123 will allow you to import a netlist in a few formats: Protel, Tango, PCB123 v2 Schematic netlist or the simple netlist that you can generate from a PCB123 layout. If you are an Orcad user you can generate the Protel or Tango formats. You will see the option to import a net list when you start a new design. The First page of the new board wizard allows you to import a netlist. You can import a netlist in the board configuration only after selecting the New option to create a new board.

After selecting the netlist PCB123 will have you select the footprints you want to use on your layout based on the entries in you netlist. You should try to use descriptive names for your parts. If you use names such as 0402 or SOIC8 PCB123 may pick parts for you from our standard libraries. After you have selected the first footprint you will see a message asking you if you would like to remember these package assignments. If you say yes, a named labeled global.alias.xml is created to store these assignments. If you say no the global.alias.xml is not created and each time you import your netlist you will be asked to select footprints. The global.alias.xml can be located in the following locations.

XP: C:\Documents and Settings\All Users\Application Data\PCB123\Lib

Vista and Win 7: C:\ProgramData\PCB123\Lib

If you make a mistake in your package selections, you can delete the global.alias.xml to start the part selection process over. After deleting the file you can import the netlist is again by selecting Design Compare Netlist/Update Design.

Once you have created design you may want to update the layout with a modified netlist. Select Design Compare Netlist/Update Design to import the updated netlist. If any errors are reported after importing your modified netlist, no changes will be made to your layout. Once you correct the reported errors you can import the netlist again and you will see your changes.

The most commonly reported error states that the part selected does not have a pin numbered #. This message is telling you that the pin numbers for the footprint that the global.alias.xml is pointing to does not match the pin numbers listed in your schematic symbol. You will want to check the footprint stored in your footprint library for the error. If the footprint is correct, you should check the global.alias.xml to see which footprint was selected. If the wrong footprint is selected, you can delete the global.alias.xml to select the parts again.

Sal