I have designed a board which is a slightly irritating shape but sadly necessary in order to retrofit,
my question is that when i want to add the GND plane to the board, do i really need to trace the outline of the board?
I have tried just drawing a box around the whole thing and it gives the desired result, but there is the hatched area where i drew the zone which is a little offputting, but does it actually affect the gerber?
the board and 3d view it looks exactly how i hoped it would
No. (OK, if you are obsessed with the appearance of your project on your computer display, then it may be important to carefully align the zone to the board’s corners, edges, etc. That task could fill up a rainy Friday afternoon when there isn’t anything happening around the office.)
The major requirements for the zone outline are:
It must be a closed contour. No gaps, or segments that “almost touch”. Same applies to your board outline (the “Edge.Cuts” contour.)
It must have a net explicitly assigned to it.
There must be a pad or trace, within the zone outline, assigned to the same net as the zone.
When different zones overlap, or when one zone encloses another zone, the zone’s “Priority” becomes significant. Search the Forum for discussions about zone priority if this situation applies. (In your example, it doesn’t apply.)
The algorithm for filling copper pours (“zones”, or “planes”, if you prefer) treats the Edge.Cut line like a copper trace, and stops the poured region just short of the Edge.Cut line. The gap between the pour and the Edge.Cut is controlled by the same “Clearance” parameter as the other traces within the pour. One of the Forum threads that gives additional insight into this behavior is " Creating “zone outlines” for odd shaped PCB’s(Or just have them to be the shape of the cutouts) "
No. You can prove that to yourself by generating a set of Gerber files and loading them into a Gerber viewer. You don’t have to wait until your board is finished to create Gerber files; just be sure the trial Gerbers never get mixed in with the final Gerbers. The process shouldn’t take more than a few minutes. (I prefer the “gerbv” viewer from the gEDA project, rather than the viewer in KiCAD, but there are dozens of no-cost or low-cost Gerber viewers that will do the job.)
For better or worse, the Gerber files are the defacto industry standard for communicating design information to board fabricators. Regardless of what KiCAD displays on your computer, or what the 3-D models show, your boards will be manufactured according to what is in the Gerber files. That is why many of us do a thorough inspection and review of the Gerber files - perhaps investing a few hours of our time - before we send an order to the board manufacturer.
(If you poke around this Forum you may find some threads pointing out that some bug-infested CAM software, used by a few low-cost fabricators, incorrectly interprets the Gerber file spec. If I recall correctly, the problems only affect silk screen layers, and show up in the vendor’s pre-order review of the job.)
