Altium design rule question

[docmur]

Hey Guys

Does anyone know how to setup a rule for the distant a VIA has to be away from a pad?  I currently have my board setup for a 5 mil spacing, but I want my VIA's to have to be placed even further away from pads, maybe like 10 mils+.  I can't see any setting or method to tell the DRC to look at that.

Thanks

Docmur

[AlfBaz]

In Design Rules under electrical->Clearance, create a new rule.

Select "Advanced(Query)" for both "Where the first object matches" and "Where the second object matches"
Click the "Query Helper" button. For the first type "IsVia" for the second type "IsPad"

Then simply adjust "minimum Clearance". You can even stipulate whether this clearance rule applies to all or just different nets

[AlfBaz]

I forgot to mention that you sometime have to give rules in similar categories priorities. For instance here you might want to give your pad to via clearance rule a higher priority to your general clearance rule

[T3sl4co1l]

Could probably also be done with IsSMTPad and hole clearance, so it applies to all holes.  Or something.