Polygon rule problem

[Korken]

Hi all,

I have been trying to get a rule for polygons working but I am unable to find my error.
I have the simple rule that vias that belong to GND should have a direct connection to the GND plane (check attached image).

But it does not work I get the normal 4-spokes connection on vias.
If I try my rule in the PCB filter box I get all the correct vias selected.

What have I done wrong?

Thanks!

[AlfBaz]

I do this and it works. If nobody provides an aswere by the time I get my PC back together, I'll have a look and let you now

[free_electron]

your rule is wrong.
you let the tool search for an object that is 'in GND' AND is a via and compare against another object that is 'in gnd' and is a via ... that doesn't work. your logic is flawed. you are setting the rule against two via's that are ground.


set your second object to 'all'


and why only do this for ground ? i simply set this for all via's connecting to a polygon.

[AlfBaz]

and why only do this for ground ? i simply set this for all via's connecting to a polygon.

Just had a look (been a while) I use IsVia and all

[Korken]

Thanks both of you!

What really got me is that I do not yet fully understand what it means to compare against another object in a rule.
Since I only have a via, I do not want it to compare against anything (I just want it to connect)? The rules part of Altium is still a bit fuzzy for me.

[AlfBaz]

What really got me is that I do not yet fully understand what it means to compare against another object in a rule.
Since I only have a via, I do not want it to compare against anything (I just want it to connect)? The rules part of Altium is still a bit fuzzy for me.

The example at hand may not be the best but generally you create a rule that applies interaction between two objects. In this case the first object is a via and the second, ALL with "direct connect" applied between the two

A clearance rule is a better example where the first object may be a certain net and the second can be everything else (ALL) or some specific other net or group of nets

[ajb]

What really got me is that I do not yet fully understand what it means to compare against another object in a rule.
Since I only have a via, I do not want it to compare against anything (I just want it to connect)? The rules part of Altium is still a bit fuzzy for me.

The example at hand may not be the best but generally you create a rule that applies interaction between two objects. In this case the first object is a via and the second, ALL with "direct connect" applied between the two

  And since polygon connect rules only affect how polygons connect to pads and vias, it's implicit in the rule that one of the objects must be a polygon and the other must be a pad or via.  You can use the second object filter for more specific rules--for instance to select only polygons on certain layers, or only certain named polygons--if you wanted some polygons to connect one way and others another.

[Korken]

Ahhhh! Thank you both for the clarification!
Now I'm starting to et a better hang of it.