I am new to this forum, so feel free to direct me elsewhere if this post is in the wrong place or this question has already been answered.
I come from a background in Altium, back when I got a free license for being an undergraduate. I have started to do open source hardware design, which I will be documenting in a blog at some point, and made the switch to Kicad. I do not expect the level of complexity that Altium has from KiCad, I am just curious!
Simply put, if you have a board with isolated grounds and multiple voltages, you will end up with many,sometimes odd shaped, copper pours. If I make a copper pour, and then move some components and now my copper pour is in the way, leaving some slivers that I donāt want. Now I want to delete a part of that copper pour, but not the whole thing. The only way I found that I can do that in Kicad is to redraw the entire pour, which can be annoying if you have 20 points to click on to create the pour. In Altium you can click on the pour itself and in the popup menu you can edit the location of the vertices of the pour, which is convenient.
Is there a better way to do this than re-drawing the pour? Or is this a feature I should suggest, and if so where can I go to suggest new KiCad features?
Unfortunately the pours are not done exactly like the traces (where you can remove certain segments at a time).
First, select the pour tool and right click over top of the pour and chose to āRemove Filled Areasā. Then when itās just the outline of the pour area once again, you can manipulate the zone using āGā (grab the zone and drag the segment around), āMā (which moves the entire pour area shape around), āAdd cutout areaā (via the right click context menu, allows you to modify the zone by drawing new areas you donāt want" or āCreate cornerā (via the right click context menu, creates more segments you can drag around using the grab command). Note that to get the āZonesā context menu you need to right click directly over the outline of the zone, which is why removing the filled area helps.
You sir are awesome. I actually think that the way that KiCad edits pours is preferable to the way that Altium does it, or the way that I did it in Altium anyway.
These sound like two different things ?
If you have issues with Zones start with a simple board and simplest of Zones, and check that works,
Then, start getting more complex, until something breaksā¦
In most CAD pgms, there is a shrink step, where the zone-border is what you draw, but the real world requires some line width is used to plot the fill, so the SW shrinks the border.
Sometimes, that shrink can fail, usually on cases where the half-width removal, results in a narrow segment trying to go < 0 length.
ie avoid very short line segments.
Not two different things at all. ChrisGammel mentions:
Iāve narrowed it down to the case where a cutout zone overlaps the edge of a pour zone.
Selecting āAdd cutout areaā puts the mouse into polygon mode (i.e. each click places another point in a polygon). As soon as I right-click and select āClose Zone Outlineā, pcbnew crashes. You can try it yourself:
Launch KiCad and create a new project
Start pcbnew
Use the Copper Pour tool to create a single rectangular copper pour area
Right-click on the pour outline, select Zones -> Add Cutout Area
Draw a polygon that crosses the edge of the pour.
Right-click and choose āClose Zone Outlineā
Poof!
Anyway, Iāve reproduced it with the latest source, so Iām off to file a bug.
Interesting - thatās only in legacy mode, but it is a slight variant of Add-Cutout
In this pathway, it acts like a nibbler, and will add slices into the existing cutout outline, if the added polygon crosses the outline. Once done, the construction line vanishes. Quite nice.
It does not seem to need an explicit āClose Zone Outlineā to work.
Works for me, Iāve nibbled into an Outline in 4 places, and also added a void inside the outline.
Seems to also be ok with a tangent case (shared side)
Tested : Win64 build. r7066
Turns out itās only an issue in a Debug build of KiCAD. I have forked KiCAD to add support for database-driven symbol and footprint libraries, so I was running a Debug build. There is an assert that fails. In a release build, everything is copaceticā¦EXCEPTā¦for me, after I make the first cutout, the āClose Zone Outlineā option in the right-click menu is gone! I canāt close another outline until I restart pcbnew. I assume that is also not a problem for you, since you described making several cutouts.
What is the āAdd-Cutoutā thing you are talking about, if not from the step-4 I described? If thereās another path that works more reliably, Iām all ears!
Hmm, what version of KiCAD are you using? My right-click menu in pcbnew does not have an āAdd Voidā entry. Iām using the latest development version, built from sourceā¦
Ah, I see. Note that what you describe is not the same thing. You are describing adding a keepout, which would affect all zones that it overlaps, and exists as a separate entity in the layout. The OP and I are looking to modify the actual pour zoneās polygon, i.e. add edges to the polygon. Thatās what using the zone tool to add a cutout zone does, and only affects the zone being modified.
Anyway, Iāve submitted my bug reports and know how to skate around the issues. Thanks for engaging, PCB_Wiz!
)