Able to assign a Net to a Graphical Copper feature?

Hi. I have a graphical feature - basically a rounded copper pour with a hollow center - that was modeled using the “Graphic Circle” tool. I placed it on the Top Copper plane however there is no net assigned to this feature. Is there a way to assigned a net to an arbitrary copper pour feature. Alternatively is there a way to pour rounded circles (with assigned net) that have hollow insides kinda like a dart board?

As soon as you want to connect a net to it, I immediately think “Footprint”.

I do not know what you mean with “rounded circles”.

In KiCad footprints are very easy and quick to make (after the initial learning curve which is not very steep either). Rectangular pads with rounded corners are one of the standard forms of pads.

In KiCad it is also common to put multiple pads/pins with the same pin number (which is more a string of text) in a footprint. All the pins with the same number then connect together as a single pin in the footprint.

For example:
First open the Footprint Editor from within a project:

Then type “thermal” in the search bar and click on one of the components to show it in the editor.

The SMD pads 1 through 10 of the component I chose have rounded corners, and pad Nr. 11 is made out of a big red SMD pad and 6 THT pins.

Thanks Paul! I was trying to avoid footprints BC I need 6 different diameter rings of copper each with a different width and a different hole size in the middle. These are basically 6 circles within circles each different sizes. If I use footprints then I have to do 6 custom footprints, one for each ring. I guess if there is no other way, then this is the thing to do… It would’a been cool if you could pour copper (and give it a net) based off another layer’s form (such as the User Drawing layer or something). Or if you could just assign a net to any arbitrary copper form.

Making custom footprints is really trivial.
Adding a custom Footprint library to a project is about 5 mouse clicks nowadays.
When you 've made the library and your first footprint, you can just copy it a few times to footprints with different names and change the pad parameters for different diameters etc.

Creating nets in Pcbnew is … not recommended to say the least. and almost always are a request for a dirty hack and more trouble than it’s worth.

Concentric circles… Ouwtch. KiCad is unfortunately still lacking complete support for circular (and arc segments) of tracks. I think (but am NOT sure) it’s coming (already in V5.99?). There are also some plugins for curved tracks. But I would not recommend these solutions to a beginner.

Creating nets in Pcbnew really is *&^%$#@! It’s much easier overall to make a (simple) schematic. for example a net that connects 2 test points together. Then if you use some of the existing SMT test point footprints:

…you also create the nets for use in Pcbnew. Once you have such a testpoint pad you can draw a zone around it to extend it.

Support for Circular things is still a bit difficult. For more complicated shapes, often an import from a CAD program (usually .DXF) can be used.

I am missing an overview of what you want to make, which makes it difficult to give better advice.
Unfortunately new users can not upload or post screenshots and first need to accumulate about half an hour of “viewing time”.

1 Like

Yes, that is an issue - I wanted to post my graphic but cannot do so. Anyway, I’ll try the custom footprint tool. Maybe that’s let me do 6 concentric circles each with varying widths and diameters and center holes. Basically I am creating a multi channel capacitive sensing “antenna” with several concentric circles. The board is circular as are the 6 “pads”. I’ll give it a shot. Thanks again Paul.

Also, how would I import a DXF file and assign nets to its parts? That could be another approach.

I promoted you one level, you should be able to post now

Thanks Dave.

Kevin Kachikian

Bard Designs

Mini Tutorial for importing dxf and making footprints out of them.

First I drew an arc in Freecad’s draft workbench:
and exported it as “arc.dxf”.

Then: Open KiCad’s Footprint editor, and create a custom library.
KiCad’s default libraries are read-only, so you need custom library.
In the new library create a new Footprint, with the IC like icon just under “File” in the left top corner:

Footprint Editor / File / Import Outlines from DXF file

During import you can select any non copper layer to put your arc on. I choose Dwgs.User:

To make a pad from the arc, it needs a “real” pad as an attachemt point. so add a pad:
Footprint Editor / Place / Pad and place it in such a way that it overlaps:

Last step is to combine these 2 shapes into a custom pad.
Press and keep pressed both [Shift] and [Ctrl] and then click on both shapes, then release [Shift] and [Ctrl]. Press the Right Mouse Button and select “Create Pad from selected Shapes”.

From your screenshot…
I’ve got some better idea’s.
I will experiment and report back shortly.

Thanks Paul. Very kind of you. I realized my drawing is double size - it should be 56mm for the board size, not 112. Not that that matters…

Your screenshot looks like it’s already a complete PCB with circular tracks.
The simplest way for you now is probably to just draw the schematic and use the “test pin” as endpoints for the net, in the way I showed in post #4.

If I would design this, I would simply place concentric circles in a single footprint in the footprint editor, and combine each circle with an SMT pad into a custom pad. If you do this you have a footprint with 6 pads that you can link to from the schematic.

I think that’s what I’ll do - just draw all that in the footprint editor. Thanks again for all the help!

You can easily adjust all parameters of a circle by hovering over it’s edge and pressing e for Edit.

So make a scetch on a piece of paper with measurements and use that to punch in the numbers.

You can also enter simple calculations in those entry boxes. 5+6 will get evaluated to 11. If entry is in mm such as in the screenshot, and you enter 4" then KiCad will evaluate to 101.6mm.
It also does not matter if you enter dots or comma’s as separators. KiCad is “international” in this regard.

Yes, that’s exactly how I created the above. Only thing is no way, that I understand, to assign nets to each copper pour. But your pad idea should do it I think.

In my mini dxf tutorial I connected a pad to custom graphics.
Each pad has a number (or more correct a text string as name).

If you name the rings in your footprint with 1 through 6, then you can use any simple 6-pin connector schematic symbol and connect wires to it in Eeschema, and link it to your custom footprint.

If you want to make custom schematic symbol that’s also possible, but a bit more work.

Oh, I see. OK. That sounds better. Will do that!
Thanks from LA…

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.