[SOLVED] Clearence between traces in Altium

[DrBudz]

Hi folks,

I have one RF trace which requires 12mil clearence. Other components and nets have 10mil clearence.
I want to place ground plane which will have 14mil clearence on the whole board, except near the RF trace where it should be 12mil.

How can I make the clearence between ground plane and RF trace to 12mil and between ground plane and rest of the traces to 14 mil?
Is there samo sintax like this:

clearence between GND_Plane and RF_Trace = 12mil
clearence between GND_plane and Other_traces =14mil

Thanks

 

[PCBcomponentlibraries]

Hi,

You need to make a few clerance design rules. Go to Design --> Rules and select Clerance right click on it and select new rule. You can then click on the new rule, and add the query add 'InNet(RF)' in the top box and 'ispoly and InNet(GND)' then change the clerance to what you desire. The attached image should help.



Oh and then set up the other rule... but I'll let you figure that one out.

 

[DrBudz]

Thaks for the hint.

It didn't worked with "IsPoly", but it works with "InNamedPolygon".
Here is the picture.**broken link removed**

 

[loosemoose]

you will need to use "InPoly" for design rules (not "IsPoly").

 

[PCBcomponentlibraries]

Yeah, sorry I get them mixed up all the time inpoly is the way to go.