KiCad for screen printed smart textile circuits?

[MarkCatchpole]

Hello!
I am the commercial director for Conductive Transfers(CT). CT is a small company that prints circuits for smart textiles including https://www.myinnovo.com/ which is a smart garment that is used to treat urinary incontinence. The CT process involves screen printing layers of stretchable insulating and conducting inks and finally an adhesive layer on to a 100cm x 70cm PET transfer film. After each layer is printed it is cured in a tunnel dryer. The circuit is finally heat pressed onto a textile such as Lycra/Spandex. This results in a stretchable smart textile circuit with no substrate.

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 using conductive adhesive onto the printed circuit prior to heat pressing. Currently we use Adobe Illustrator to do the circuit artwork. However as our circuits get more complicated this is becoming unsuited to the task.

KiCad potentially looks like a good option for us going forward, but before we dive in I have some questions:

1. Has anyone else used KiCad for designing printed circuits? If so, how did it go?
2. Is it possible to easily create sinusoidal/wavy tracks?
3. Is it possible to create a custom layer stack similar to the above that allows DRC checks?
4. Printed circuits don’t have vias as such - you get them for free by leaving a hole in a dielectric layer and printing a layer above. What is the best way to handle this with KiCad? Will this be ok from a DRC/LVS perspective?

Kind regards

 Mark

[poco]

Probably it would be useful to see some example files to be created (how these wavy tracks should look like?). KiCad cannot create sinusoidal tracks, it supports only arcs ant straight line segments). Also, what output file formats would you expect? Pcb Editor can run python scripts, so maybe, script could convert ordinary (straight) tracks to wavy (lines + arcs) or sinusoidal (only line segment approximations) ones.

[der.ule]

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:

Post-v5 new features and development news

@ArtG @craftyjon Yes, the reason is that I had anti-aliasing disabled since my machine is a little slow. Please see video below with “Subpixel anti-aliasing (High Quality)” enabled as well as the newer KiCad color theme. Fillet_Tracks_AntiAliasingOn

Post-v5 new features and development news

Corner rounding is back, working better now arc_placement_3 Note: this is just for placement of new tracks. Dragging around and shoving existing tracks is separate, and still has issues with rounded corners.

[MarkCatchpole]

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.
Regards
Mark

[MarkCatchpole]

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

[poco]

You probably want to use length matching feature, see 5:10 https://youtu.be/chejn7dqpfQ. 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).

[poco]

All in all, you shoild download kicad and try it out, it will not hurt you . 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.

[MarkCatchpole]

Simple example of printed tracks best seen in adobe acrobat so that you can turn layers on and off:
https://wearableconsultants-my.sharepoint.com//p/mark/EQRVbtv67QVCniflhK2g9-ABs0Y6WJ-HCRvAP_b3aOSa7A?e=Cs0htP

[MarkCatchpole]

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

[hermit]

@MarkCatchpole

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.

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

[MarkCatchpole]

Thanks for the upgrade

[eelik]

@MarkCatchpole

• Is it possible to easily create sinusoidal/wavy tracks?
• Is it possible to create a custom layer stack similar to the above that allows DRC checks?
• Printed circuits don’t have vias as such - you get them for free by leaving a hole in a dielectric layer and printing a layer above. What is the best way to handle this with KiCad? Will this be ok from a DRC/LVS perspective?

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.

[der.ule]

@eelik

However, there’s no real limit how layers can actually be used

???

32 Copper layers and 10 user layers AFAIK.

[eelik]

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.

[der.ule]

Another example of wavy stuff:

(V6) PCB Editor: rough edges on copper pour

@JeffYoung, many thanks, this was exactly what I was looking for. I’ve set it to 0.001 and the results are better, though not ideal. Apparently KiCad won’t go lower than 0.001. As suggested in the first reply, KiCad changed to using arcs would be ideal solution. @BlackCoffee, yes, as you’ve already said, your remark is snarky. And patronizing. I have the impression you haven’t even understood my initial post as the rough edges lead to misclassification of the board, leading to higher cost. If t…

[MarkCatchpole]

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.

[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.

[MarkCatchpole]

Thanks so much for your detailed reply and examples.

[paulvdh]

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.

[eelik]

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