Hello all,
I am getting a warning stating this:
Copper connection too narrow (board setup constraints minim connection width 5 mils; actual 4.25 mil)
I think that this is a setting issue. The board has tight tolerances. In my copper pour settings I selected the minimum to be 5 mils. So it looks like that it is making something 4.25 mils which is incorrect
Again, I think that this is a settings issue. Any thought on how I can fix it?
I suppose somewhere there is too little clearance and the filling on both sides only reaches each other with the tips.
Without seeing or knowing more about that something it’s difficult to say. Piotr’s guess is good but we can’t validate it. You could find the DRC marker, zoom to it and show in a screenshot what it points to.
Also you don’t tell your KiCad version (Help → About → Copy Version Information button). This may be a bug which has been fixed.
It looks like it could be a bug. You should try with v9 if the problem persists. Or at least 8.0.9 which is the last bugfix version of v8.
You can also zip and attach the project here so that someone else can try.
So unfortunately, I don’t think that my client would appreciate sending a zipped copy of their board out to the internet…
I updated to the latest version of KiCAD (9.0) and I am still getting that issue.
Been there and (not) done that.
One idea…is the area in question just a small piece of a much larger board? Maybe copy to a new project and remove 95% of it (all but the area of interest, update from the pcb to the schematic) ?
Looking at your image, I cannot tell that connections are so narrow. I seldom do anything less than 10 mils wide…but I am doing power so connections to a fine pitch controller IC will be narrow.
While this may be perceived as a bug (Why would KiCad ever pour smaller than the minimum copper width), this is helpful to see in some cases.
The Zone minimum width will give a rough, 99% good solution that is guaranteed not to violate clearance. However, in tight tolerances, this may result in the fill being reduced below the minimum copper width set in the board setting (in order to ensure we do not violate clearance).
The DRC check exists to inform you of this situation. You can move elements on the board to adjust the fill discrepancy or you can change your minimum width in the board-level setting. Since violating clearance is generally more dangerous than violating minimum width, we tend to error on this side of the equation at the moment.
For me it is exactly what I had in mind. There is just not enough room to route there 5 mils track so tracks from both sides touch each other with their rounded ends as far as possible and in its thinnest point the connection is less than 5 mils.
At the place with 2 arrows you can move the track on the right probably 1 mils and you will get better connection between both filled parts.
I see thanks guys for your feedback. I did play around with the minimum width and was able to get most of the warnings to disappear. There is a small handful but for those, I might just move the traces a bit to clear them.
