Altium designer rule set for power nets

[Jonathan]

Hi guys,


How do I make a rule set for the power nets?

I want the width and thickness of my PCB power nets automatically been set to the design rules.

So that i don't have to manually adjust them all the time.

[budi]

Hi Jonathan,

To set design rule, it can be done in schematic and PCB.

Normally if the design flow is from schematic then to PCB, we can set PCB design rule from schematic by placing "directives".
To set new width rule, you can place "PCB layout" directives ( Place >> Directives >> PCB layout ), then edit the rules on that directives.
before you place it on the schematic, hit "TAB" key on your keyboard, and new setting window will pop up. click "add as rule" button continue to click on "edit rule values" button. after that, to set the width of the track, double click on "width" rule and set the track's width.
then click OK to close the window. place this directives to your power net i.e, GND and VCC.
Every Directives that you placed on the schematic will create one design rule in PCB file.

In-case you don't have schematic file, you also can set the design rule from PCB file.
To set it, open PCB file, select "design >> rules"
search for "Routing >> Width", expand the rule by clicking on the "+" sign. if you use default PCB setting from Altium. it will automatically create one "width" rule, when you click on it. it will show the setting for All nets and default rule for min, preferred, and max width is 10mil.
To create new width rule, right click on the "width" and choose "new rule". Altium will automatically create one new width rule with the name "width_1". click on that new rule, on the right side, you can change the rule name. to set this rule for particular net, Choose "Net" on the "Where The First Object Matches" and from the drop down menus, choose the net name (example: GND, width:50mil). after that, change the track min, preferred and max width.
click "Apply and OK"

And now, when you route GND net, it will automatically place 50 mil track.

To set the thickness of the trace/copper, select "Design >> Layer stack manager" and double click the signal layer (i.e top/bottom layer) and then set the copper thickness.

Please let me know if you encounters problem during the setting.

Regards
Budi