How to Remove Pins From a Routed Board Net?

Question

Hello all,

I had submitted this question to Richard in Cadsoft support, but thought I start it as a new discussion as well.

I have a simple issue that I'm stuck on. I've finished routing a four layer board, and somehow managed to connect a chip enable net, N_CE0 to the power plane net, VDD_FLASH. I need to remove two pins from the power net and recreate the chip enable net. I've tried deleting the routs and airwires for the chip enable net, and entering the netlist again with no luck. Can you tell me how to correct my problem?

Thanks in advance for any help you can provide.

Cheers,

Ralph

Former Member · Accepted Answer

Hi,

I am not sure if the connections are to supply plane or to a polygon, so I will provide you some simple steps you may consider.

Supply Layer

If you are using a supply layer, use the DISPLAY command to view your layers. You will notice your internal layer will have the name $VDD_FLASH. Double click this layers and disable the SUPPLY option and click OK and run RATSNEST. You will now notice the airwire. In the schematic, delete the connection and make necessary modifications. If you are using a SCRIPT file, delete the connections on the board and import the script file or use the SIGNAL command to define the coneection manually.

Polygon

Type the command RIP @; and press enter. This will ripup all the polygons and place them in outline form. Now click on Options/Set/MISC tab and disable the option 'RATSNEST PROCESSES POLYGONS'.

Now run the RATSNETS command. You will notice the the implicit airwires appear since the polygon no longer pours. Make the appropiate changes to the schematic. If not, delete the connections on the board and import the netscript.

I hope this helps.

Best Regards,

Ed