How to make round zones for Gnd and +5V etches

[joesilva1]

Back about 2 to 3 years ago I made round PCBs. I have forgotten how I made them. Here is a picture of the PCB I made in the pass. How did I do this? I cannot believe I forgot.

Thanks in advance,

Joe

[paulvdh]

Your image link did not work, I fixed it by removing a space in between the [image] and the (link:).

KiCad does not support real circles and arcs as zone boundaries, but your thermal reliefs suggest that you do nave real zones. That is a bit of a puzzle.

[maykol_rey]

I tried it directly in Kicad and I couldn’t do it, I think the best thing is to use Inkscape and from there import the shape you need.

[paulvdh]

Meh, you’re giving up too quick.

[paulvdh]

I’ve got something working.

The simplest way would be to directly draw graphical objects on copper, and add some pads. But that’s not a nice project. KiCad V8 does have the ability to assign net names to graphical objects on a copper layer. But that is new in KiCad V8. You could not have used it in your old project.

For the above screenhot (and your project).

1. Create a schematic with all nets and footprints. Maybe 4 testpoints for the 5V net, and 4 test points for the GND net.
2. [F8] them to the PCB so you have the footprints and nets.
3. Select Edge.Cuts and draw the circle for the outline.
4. Draw a GND zone around the PCB. It will be clipped by the circle on Edge.Cuts.
5. Make sure a footprint with the GND net is in the proper place, so KiCad knows how to fill the GND zone.
6. Draw a circle on the margin layer. You can experiment with line width to get the clearance you want.
7. Draw a new zone. Just a rough polygon and about the same size as the circle on the margin layer.
8. This new zone must have a higher priority.
9. Put the +5V footprints inside.
10. Draw another smaller circle on the margin layer.
11. Cleanup and make it pretty.

I put a random footprint in the project, just to have something solid to connect the nets to.
I’ll attach the file so you can look what’s inside it.
00aa_module.pretty.kicad_pcb.zip (21.8 KB)

A third option is to:

1. Create a circle on a copper layer.
2. Select. Right click and then: Create from Selection / Create Polygon from selection and use the Create Boundary Hull function.
3. Use this function again, and now turn it into a copper zone.

This does not give you an exact circle, but a pretty good approximation with line segments of a round zone. You can set the accuracy in: PCB Editor / File / Board Setup / Design Rules / Constraints / Arc/Circle approximated by segments: Maximum allowed deviation: …

[maykol_rey]

This is how I did it using Inkscape!

[paulvdh]

@maykol_rey

This is how I did it using Inkscape!

You don’t need Inkscape for that. You get that result by just drawing graphical circles on a copper layer in KiCad. Now add the thermal reliefs, and the pads that extend beyond the inner circle of the zone. That is why I added the third option to draw it as graphical shapes last.

[joesilva1]

Thank to all, I believe I know what to do now.