KiCad for screen printed smart textile circuits?

KiCad (v6) has some support for wavy tracks, it is quite a new feature but I may be enough for your needs, if it isn’t, poco’s idea of scripting is feasible:

1 Like

Hi Poco
Many thanks for your reply. I just tried to upload a pdf file to show you an example but as a new user I was blocked.
I would like to output each layer as a pdf.

Thanks for your reply and pointing this out. I will look at wavy track support first.
Kind regards

You probably want to use length matching feature, see 5:10 All your tracks should be like these rounded meanders, I think. You could share pdf via google drive untill moderators will raise your status. Youtube video is from v5 (outdated version of kicad). v6 is released a month ago, and probably does not have such video help (controls can be slightly different from v5).

1 Like

All in all, you shoild download kicad and try it out, it will not hurt you :slightly_smiling_face:. Exact program to be explored is called PCB Editor. Kicad has several other executables as a package, Schematic editor is for creating schematic. You should explore pcb part first.

Simple example of printed tracks best seen in adobe acrobat so that you can turn layers on and off:

Agreed - I have just downloaded it to have a go
Thanks again.

1 Like

Sorry about that. It as an anti-spam feature built into the software. You’ve been ‘leveled up’.

Thanks for the upgrade :grin:

Tracks can surely be created by scripting, as was already pointed out. There may already exist some script, and if you ask nicely or are willing to pay, someone might write a plugin for that purpose.

KiCad has a layer stackup manager, but it’s meant for boards. However, there’s no real limit how layers can actually be used. As long as the manufacturing software can handle gerber files, it’s pretty flexible.

I don’t see vias as a problem. Just use small vias, smaller than the track width. You don’t need the drill files anyway (I suppose), and the extra copper features coming from vias would be inside the tracks and shouldn’t matter. As a last resort vias can be deleted before exporting to gerber.



32 Copper layers and 10 user layers AFAIK.

I meant for manufacturing. Layer names are only conventions. EDIT: KiCad may add some layer data to gerber files which can be interpreted by a proper software, but especially user layers are just graphic layers and the software should be able to use them as they wish.

Another example of wavy stuff:

1 Like

Thanks for your thoughts on this. I think it is definitely time for me to do a trial. I am reassured that it is possible to script a solution if necessary.

A simple screen capture of the intended layout:

KiCad is a PCB design program suite ( Printed Circuit Board :slight_smile: )
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:

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.

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.


Thanks so much for your detailed reply and examples.

I just noticed a sharp corner in your design:


Such corners rise the stress in the material during bending and those are often a place where cracks start. This is a very big concern in Flex PCB’s. I do not know much about the materials you use, but avoiding such corners is likely to result in a longer life expectancy of your product.


In the future teardrops (under development and testable in nightly builds) can take care of this.


Thanks for pointing this out. For our printed inks this probably isn’t critical but I agree that would be better to avoid it.

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