Hi,
I made the following settings:
but the clearance between track and GND Plane is still 0.2mm. I actually modified it to 0.15mm as you can see. After this the CMD+B command was pressed.
Can anybody tell me why it is still 0.2mm?
Have you tried to move the track after changing the minimum clearance value? Just reducing the clearance does not immediately change the location of existing tracks.
Maybe it’s just on a grid?
1 Like
Did you remember to recalculate the copper fills? I forget exactly what the menu item is called, but it is keyboard shortcut “b”.
1 Like
Copper fills have their own clearance. You can only increase the clearance to a track compared to the zone clearance not reduce it.
1 Like
But the grid shoudln’t be important for the distance from track to ground plane? Its the distance to the groundplane which wonders me. The distance from track to track ist still 0.15mm.
Yes, I reculculated the copper fills via b
Would this mean:
track clearance+zone clearance=clearance from track to zone?
But I don’t think so because track clearance is 0.15 and GND Zone clearance is 0.15
so in total 0.30 which is not equal to 0.2mm . Is there any clearance setting I still forget?
It is not an addition. It simply that the zone clearance and the track clearance are both minimum constrains and if you combine two minimum constrains then the larger one of them wins.
So if you set zone clearance to 0.1 but track clearance to 0.2 then the resulting clearance will be 0.2 but if you set zone clearance to 0.2 and track clearance to 0.1 you still get a clearance of 0.2.
1 Like
OK, nice. What happens if there are more than one netclasss with different clearances. Does it use the
“worstcase” ?
Clearance GND Zone =2
Clearance Track 1 =0.5
Clearance Track 2=1.5
Clearance Track 3=2.25
->Result: Clearance from Track1 to GND Zone is 2.25 ? Is this the way it works?
No the clearance is calculated for every trace independently. So if one trace has a clearance of 0.2 but the other of 0.3 then both of them get the clearance as set unless the zone clearance is larger than either of them.
1 Like
When I measure in my Layouts this isn’t the case. There seems to be a difference of 0.05mm.
You also cann seein the screenshot above.
Is it possible that the net that your zone uses is in a netclass that has a larger clearance requirement than you set in the zone?
2 Likes
Yes, thats the reason! Thank you so much for helping me! GND was also declared as Default and Default was 0.25mm. Important to know clearance from zone to track = Maximunm (clearance track, clearance zone properties, clearance net zone).
I added an screenshot for logic reason. But topic can be closed now.
And thanks to all the supporters of the KICAD forum.
1 Like
It just could’t be another way - it is as 2x2=4.
Any clearance setting not specifies the exact distance (PCB could not be designed) but the minimum distance. To satisfy several such minimum conditions the distance between considered elements in any point have to be greater then the maximum of all applied conditions.
If you have a high-voltage net and you specify for it huge clearance (say 1cm) then you expect to have that distance to anything else even if that second element has its clearance set to 0.2mm.
2 Likes
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.