KiCad for screen printed smart textile circuits?

[paulvdh]

A simple screen capture of the intended layout:

KiCad is a PCB design program suite ( Printed Circuit Board )
KiCad is very limited in it’s graphics capabilities. It’s main tasks are with working with schematics, parts on schematics, Footprints for IC’s and the copper connections between them, and at the end, generating Gerber files, which are a standard file format for PCB manufacturing.

KiCad is very good at controlling the width of copper tracks, and maintaining specified clearances between different nets.

Another concern is the output format of KiCad.
The usual format for a PCB are a set of Gerber files, but KiCad does support some more formats.
A list is in: PCB Editor / File / Plot / Plot Format …

Arcs have been problematic in KiCad for a long time, but quite recently some functions for drawing circular copper tracks have been added.

Below an attempt to create your wavy track:

1. First set KiCad to “all angle mode”: PCB Editor / Route / Interactive Router Settings
   

   

2. Set the grid to something coarse, but suitable, I just used 1mm.

3. Draw a zig-zag line by counting grid points: Here I placed them on 10 by 4 grid points:
   

   

4. Select them all, Right click and select: Fillet Tracks from the popup menu:

   

5. After some experimentation, I thought 1.5mm looks quite reasonable.
   

   

This is close to the maximum of what you can do concerning “wavy lines” in KiCad. The meandering that poco mentioned is a built in function that is optimized for generating a certain track length. It only draws 180 degree bends. The method I described you can control the angles and the bend radius separately.

If you have a programmer in your team, then a scripted approach as mentioned earlier may be a good way. See for example this older topic on the forum:

Code to write sine/cosine curves for angle sensor

Previously users (@rolfo, @Pererva sorry others, new users can only tag 2) discussed how to generate a repeating sinusoidal pattern on a PCB for inductive angle sensors. That thread has now closed due to age, but I wanted to post my recent work. Here is the old thread: I have written some simple python code which generates a PCB along these lines. It does not generate a complete sensor PCB yet, but it should serve as a jumping off point for anyone interested in this kind of thing. And you m…

KiCad’s native files are quite easy human readable text files, and also easy to generate (partly) via a script. SVG files are however also easy to generate by scripts. Any program that can work with SVG files can then be used for further processing.

Adding the other features such as the circle at one end and the rectangle with rounded corners are standard features of footprints and pads, and those are not a problem.

Just for completeness I mention SVGtoShenzhen It mainly is a tool for working with SVG graphics in the KiCad context.

GitHub - badgeek/svg2shenzhen: Convert Inkscape SVG drawings to KiCad PCB and...

SVG2SHENZHEN (INKSCAPE TO KICAD)

@MarkCatchpole

Recently we have started to develop so called hybrid circuits which are the same as above but surface mount chips and other PCB components are attached

This is an area where KiCad excels in. It is designed for things like that.
If this is a mayor part of your design, then KiCad may be a reasonably good fit. If a mayor part of the design is accurate graphics layout, then a technical CAD program is probably a better choice.