EEVblog Electronics Community Forum
Electronics => PCB/EDA/CAD => Altium Designer => Topic started by: AlexBorro on August 16, 2018, 12:33:26 pm
-
I'm struggling trying to build a routing width rules to a single component.
Exemple: The resistor R1 has one pad on the NetClass "HighCurrent". There is a Routing Width rule for this NetClass to make the track 3mm wide.
But for this particular resistor I want the track to have just 0.3mm. I tried to add a higher priority Width constrain scoping this resistor but it doesn't work.
I tried: InComponent('R1'), HasCompParameterValue('Case Code','0805'), and a few other with no success.
The altium seems to ignore component scoping on Routing Width rules... I think it just cares about rules scoping nets, netclasses and layers..
Anyone confirm this and/or has any clue how can I do that?
Cheers.
Alex.
-
Make a different net for that resistor with a net tie.
-
Thanks @voltsandjolts, that is exactly what I'm doing to solve the issue. But I was playing with the rules scope trying to solve the issue without netties. But I think there is no away.
Cheers.
Alex.
-
Tracks and polygons belong to nets, not to components, so I don't think there's a good way to do what you want. You can probably construct a rule for the track segment that is touching or within a certain distance of the pad in question, but it would be difficult to codify where Altium should stop applying that rule and start applying the other. You could use a room or a region to define an area where the narrower rule applies, but then you have a room or region you need to move around with that resistor, which is kind of silly.
-
Try From-Tos. I haven't used them myself but it may be what you're looking for.
Otherwise, use a net bridge, positioned in the wide net, tapping off to a thinner net local to the net bridge and the resistor. (If you don't know what net bridges are, check out the article on that too, it's pretty instructive.)
Tim