Proper way to exclude copper pour from an area

Making PCB Layouts, Manual routing, Auto-routing, Copper pouring, Updating from Schematic, Manufacturing Output
Post Reply
Message
Author
kolyur
Posts: 1
Joined: 14 Sep 2022, 02:06

Proper way to exclude copper pour from an area

#1 Post by kolyur » 14 Sep 2022, 02:26

This question seems like it should have a simple solution but I've searched the forum and haven't found a clear answer. I have a copper pour over my whole board, connected to the ground net. On one particular component I need the pour to be kept farther away from the pads. I created a Route Keepout around the component, which did keep the pour away but it also prevents me from running traces to the pads (at least, not without generating DRC errors which I'd like to avoid). I tried making a second overlapping copper pour over just that component, with the idea that I could set the pour clearance higher in that area. However, it kept giving me an error that the pour could not be generated regardless of how I set the priority values--I'm a bit confused about how overlapping pours work and whether that's even a recommended practice. I did read about using net classes to set the pour clearances, but that doesn't seem like a solution because I only want the larger clearance applied to one component, not to other components where those same nets may connect. Am I missing something?

Tomg
Expert
Posts: 2028
Joined: 20 Jun 2015, 07:39

Re: Proper way to exclude copper pour from an area

#2 Post by Tomg » 15 Sep 2022, 02:36

...I tried making a second overlapping copper pour over just that component, with the idea that I could set the pour clearance higher in that area. However, it kept giving me an error that the pour could not be generated regardless of how I set the priority values...
1) Set the original pour's Pour Priority: to "1" (the higher the number, the lower the priority).
2) Create the second pour around the component, set its Pour Priority: to "0" (highest priority), disable (uncheck) the [ ]Use Net Clearance option, enter the desired value in the Clearance: text box and click on the [OK] button.
3) Update the pours (main menu: Objects > Update All Copper Pours) and you will see the new copper pour's clearance setting take effect around the component.
cpcs1.png
cpcs1.png (11.02 KiB) Viewed 347 times
Unfortunately, DipTrace (v4.3.0.1) pour algorithms appear to favor the smallest clearance setting when connecting one pour to the same net as another. In the following example, the smaller clearance setting of the original copper pour overrides the larger, manual clearance setting of the new, higher-priority copper pour....
cpcs2.png
cpcs2.png (10.14 KiB) Viewed 347 times
Since the two pours differ in priority one would think other characteristics that differentiate them should remain separate. If this annoying (to me) clearance settings behavior could somehow be eliminated, then the results you desire would be possible.
Perhaps someone else on this board can add more insight here or come up with a better way to do this?
Tom

octal
Posts: 52
Joined: 08 Jan 2012, 23:55

Re: Proper way to exclude copper pour from an area

#3 Post by octal » 25 Sep 2022, 23:56

The only way I found usable for that is to create (like @Tomg proposed) a copper pour with priority 1 for the poured region, and create a second copper pour for the region to be excluded and set its priority to zero. Then, all I do is set the second pour plane (with zero priority) state to unpoured (via context menu).
Keep in mind that if you do an "Update All Copper pours" command, you need to set the exclusion plane state to unpoured manually!

I think the easiest solution Novarm can propose to this pb is to add a "no-fill" kind to the "Fill Characteristcs" patterns proposed.
I don't know all the side effects to this solution (mainly on DRC) but it may solve this problem for a lot of us.

Post Reply