How to swap the via Net Name?

Question

Hello, 
 In my design have some via from L3 to L9 with multiple layer its connects with NetNames A (but its not connected to bottom layer) , I just want to connect to NetNames B, so I delete the L3 cline, those via is connected to adjacent layer GND or power shapes. 
 suppose I delete the cline in L3 is it possible those entire layer via back to "not on net name"? later I can connect to NetNames B or C? 
 as of now I have selecting those via and assign to new NetNames. its take more time Any solutions for this?

Tyler · Accepted Answer

You cannot directly do what you're asking, no. You can't force a via to be not-on-a-net. By default, vias will inherit the net of whatever overlaps / "shorts" to them. What you CAN do, however, is add the RETAIN_NET_ON_VIA property to the vias, so that they retain the original A net assignment even when you delete the clines, rather than the via jumping over to the GND plane's net. 
 After you routed the net B/C traces to where the via's connect point is, if you removed the RETAIN_NET_ON_VIA property on the via and did a move 0:0 get it to check for new connections and it should favor the signal net over the voltage net for you. 
 Or, as a final option, you could use SKILL after you were finished adding the new connections to find the shorting DRCs in the design (which should be between the via, still on A, and the new cline) and from there run the axl function to change the net on the via (and remove the property at that point if you wanted to).

Stats

How to swap the via Net Name?

Community Guidelines