I am trying to use polygon to draw tracks, and after drawing the solid polygon shape I found I can create copper zone from the shape, what’s the difference between using the shape as wire and using copper zone as wire? Does both works?
What do you mean by “as wire”? Do you mean “to make electrical connections”?
I would think (??) that if KiCad recognizes the shape as a zone, it should be the same. A zone:
- Should be selectable as a zone according to the selection filter in the lower right.
- It should have an assigned net.
If it is physically connecting two or more pads/vias/tracks but does not have an assigned net, then I think you would have a “net tie”. This is useful under special circumstances but it should not be used in place of a zone.
Does that help?
For further discussion, please be sure to go to help>about>copy version information and paste it into your next post.
Thanks for replying, yes I mean electrical connections.
Based on the selection filter the shapes are ‘Graphics’ and cannot be selected as zones, but when I use net inspector they do have correct assigned nets, does this mean they are valid connections?
And btw what is the standard way of making irregular shape tracks in Kicad?
I am going to ask someone else to “bail in” to this thread. I am unsure about full answers to your questions. But I repeat that it may be helpful to include your version information…
I think your graphic polygon on a copper layer can be assigned a net but they don’t have many properties of zones. For example if you were to move a trace not on the same net running through a zone and then refill the zone, it will be reshaped to avoid the trace. And if a pad were to be changed to be on the same net as the surrounding zone, then it would acquire thermal reliefs. And the priority levels. And so on.
1 Like
When I was learning to use KiCad shapes at PCB couldn’t get a net. Since some version (may be 8, may be 7) they can, but I have never used it.
Zones have all possibilities they had since always - they can adopt their shape to the situation found on the PCB maintaining the required clearance from copper having other net and making required connection (solid or thermal relief) to pads having the same net as zone.
Shapes are simply shapes without any intelligence built-in them.
1 Like
In KiCad V8 graphics can have a net name and be part of an electrical connection, but they are more “static objects”. A graphic polygon will keep it’s shape the way you draw it. Copper zones are dynamic regions. Thy adapt to the room there is available. For my GND zone, I usually draw a pentagon or some other irregular zone outline around the PCB. KiCad then maintains a nice clearance from Edge.Cuts, and from any internal objects on the PCB.
It’s a bit similar difference between tracks and lines (when both used for electrical connections). Lines do not get moved by the interactive router, while tracks are more dynamic and can get pushed aside (while maintaining the electrical connection).
3 Likes