1
\$\begingroup\$

I have a complicated guard ring of sorts that surrounds a network of pads and traces. This guard ring is/was connected to the GND net. I had to make so changed and reload the net list. As a result the guard ring traces were orphaned and no were longer marked with the GND net. As a result, the router will not allow me reconnect the trace ring to GND. There would be considerable work to redraw all these traces.

Is there a way to apply a net to an unconnected net of traces that is not part of an existing net?

The red circle in the image below indicate where I am trying to create a connection between the net with no name around the pads on Col7 and the GND net around Col8.

Red circle shows where I would like make a connection

\$\endgroup\$
6
  • \$\begingroup\$ If you had a screen shot it would help, but you should be able to just start a trace on ground and draw it over to the guard ring. It will violate your drc but that may not matter to you. \$\endgroup\$
    – Matt
    Dec 21, 2015 at 16:15
  • \$\begingroup\$ Yes, that was my plan if I couldn't find a proper solution. \$\endgroup\$
    – Ben
    Dec 21, 2015 at 16:20
  • \$\begingroup\$ Added image for clarification. \$\endgroup\$
    – Ben
    Dec 21, 2015 at 16:26
  • \$\begingroup\$ I think the correct way is probably to make a symbol/footprint for it. Now that that ship has sailed I don't know another way than to turn off drc. The problem is that every trace is assigned to some net name and I don't think you can edit that from layout. \$\endgroup\$
    – Matt
    Dec 21, 2015 at 16:26
  • 2
    \$\begingroup\$ Hasn't the guard ring got properties that you can edit? Shouldn't one of those properties be a netname? I don't know kicad but every PCB tool I've used of late has that feature. \$\endgroup\$
    – Andy aka
    Dec 21, 2015 at 18:18

2 Answers 2

Reset to default
4
\$\begingroup\$

I found a workaround of sorts.

  1. Disable DRC influence on routing (I selected "Highlight collisions" from "Routing options" dialog)
  2. Create a trace segment to connect the two nets
  3. Save the file and close pcbnew
  4. Reload the pcb file. pcbnew will update all the segments to the connect net.
\$\endgroup\$
0
\$\begingroup\$

In three steps (in kicad 4.0.6 anyway):

  1. Disable DRC influence on routing (Preferences->General->Options->Enforce design rules when routing)
  2. Create a trace segment to connect the two nets
  3. Tools->Netlist->Rebuild Board Connectivity

(I won't comment on concepts like inductance or that just labeling it GND won't magically keep it at a uniform voltage. :-)

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge that you have read and understand our privacy policy and code of conduct.

Not the answer you're looking for? Browse other questions tagged or ask your own question.