Your article quietly assumes that there is a full layer for said plane alone. Either add a section on how a full ground plane (as an example) can be “simulated” in a two layer setup or add a clear disclaimer about which usecases are handled at the top.
And please add your article to the FAQ index thread.
Do you mean using vias between layers so that the zones are continuous between layers?
Yes. Additionally a good idea is to limit one layer to horizontal connections and the other to vertical connections to make it more likely that this produces a near uninterrupted plane spread over both layers.
Another approach is to limit traces and components to one side as much as possible leaving the other layer nearly intact for a ground plane.
Most importantly i would point out that any approach for a dual layer board has its limitations. That it requires much more thought from the designer to ensure there is a good current return path for critical signals.
And then give the easy way out with an uninterrupted zone on an inner layer. (Why should one even use the more expensive option of a 4 layer board?) Possibly mention that through hole components with fine pitch or vias placed in a row can also negatively impact such a layer.
And yes of course this will convert your topic more to a lecture about the use of planes and their benefits rather than a only answering “how is this done in kicad”. (Only answering how to do it is a restriction of the official documentation that needs to be short. A forum post can go a bit further and also answer why one would use this feature at all)
That’s true. At the moment I would rather limit the scope.
In a lecture also isolated areas and unwanted antennas should be considered. They seem to come up often when people ask for feedback about their first designs.
I have a comment about the last sentence in the FAQ.
For the internal layers, dropping a via on the associated net will do the same as a THT pad.
[soap-box=“SembazuruCDE climbs on his soap box and expounds:”]
Yes, there is a categorical and functional difference between vias and THT pads:
[/soap-box]
That said, I don’t think the scope of this FAQ entry covers the differences and similarities between vias and THT pads, so simply mentioning both would be appropriate. Without mentioning vias you can confuse users who are designing a fully SMT board that they will need to unnecessarily put a THT component (even just a THT testpoint) where dropping a via is all that is needed.
I think you’re right to limit it to a how this works in KiCad explanation.
What a power plane is and why you would use any of its variations is another and more complex discussion.
Robert
Chris, as a non-native English speaker I cannot understand if you want to espouse a via or a THT pad 
Good call. I misused that word. 
So much for trying to be clever. 
I meant “expounds”… Going up and fixing it.
Actually, based on my tests, there’s no difference between inner and outer layers. A via must first be connected to a pad. If you create two zones in two layers in an empty board file and connect them with a via they won’t be filled. If you connect the via to a pad with the same net with a track they can be filled. Also connecting a zone where the via is counts. So, the via must be connected to a pad directly or indirectly to trigger filling.
I have edited the article. Because planes a made with zones it actually became also a short introduction to zones, which isn’t a bad thing - especially filling zones may cause headaches to novices.
Or to another zone of the same net (new feature of v5. Stitching via support)
The point is that it must be connected, possibly indirectly, i.e. through a zone which is connected to a pad. It’s a bit difficult to explain it clearly and shortly although the logic is clear. If the via connects two zones which both couldn’t be filled by themselves without that via, the zones can’t be filled even with that via. Filling is kind of propagated through tracks and vias but it must start with a connected pad.
I will come back to the wording later and try to make it clearer.
When laying out a board I always explicitly place thin traces between component pads (or vias) within a zone. (When the zone gets filled, the traces get absorbed into the zone without any visual indication that they are present.) This approach confirms that the necessary connectivity does, indeed, exist and I wont be left with unfilled regions, or isolated islands in a zone.
Dale
This might give you a bit of inspiration Filled Copper Zones not showing up in Gerbers/Printouts/3D view
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.