Designing Custom Flex Sensors in KiCad

insultcomicdog

I'm a first time KiCad user attempting to design a custom trill flex sensor using the trill flex tutorial.

I've installed the trill schematic and footprint libraries.

I'm using KiCad 9.0.5, so some of the features and UI are different than the tutorial instructions.

1) I set corner smoothing to one of the pads with fillet radius 2, but there is no option to export settings to other zones. If I click ok for selected pad, the corners are not rounded. Also none of my pads are green like tutorial.

2) When I try to connect pads to nets, if I click on a single pad there are no 'nets' available in the window that pops up like in the youtube tutorial.

I realize my questions are probably more suited to a KiCad forum but thought I post here since it seems others are having the same issue following the custom flex sensor tutorial.

See screen shots here.

Should I be using an older version on KiCad for this?

max

Using the latest version of KiCad should be fine. There have been a lot of improvements to KiCad which make things easier.

1) You need to draw the outline of the flex PCB on the Edge.Cuts layer for the zones to be filled with copper. Press the B key on your Keyboard to fill the zones. The B.Cu layer has a green colour in the video tutorial, but it is blue in current KiCad. You are right there is no more option to export the settings to other zones and the new properties pane does not have the corner smoothing options yet. Either go through them one by one or set the properties on the first one and then duplicate that zone.

2) That's odd, If you have placed the symbol in the schematic, and updated the PCB from schematic, you should have the nets.

We should update the tutorial for a current KiCad, you can now even draw the shape in something like Inkscape, import an SVG to KiCad and connect nets to individual shapes.

insultcomicdog

max

Thanks for your tips. Drawing an outline on the Edge.Cuts layer solved my copper zones. The reason why my nets weren't showing up was because 'Hide automatically generated net names' was checked by default.

Being able to import an SVG or DWG would be a game changer for me because I'm more proficient in designing them in something like Fusion360 than KiCad.

insultcomicdog

This is as far as I got today.

I can't assign more than 1 net to the ground plane. And for some reason I can't route a trace from the net that is assigned to my ground plane.

I drew my connections to pads with vias, but the pads are still displaying as unconnected.

When I run DRC I get lots of edge clearance violations.

insultcomicdog

Here's my KiCad project file.

customeflextrillsensor.zip

297kB

giuliomoro

I don't see the airwires when using zones. However I do see them when using the rectangle instead. Rectangles can be filled and have filleted corners, so you could replace your zones with rectangles and it should work?

giuliomoro

No wait, rectangles can't have filleted corners ... that's annoying. There's no airwires for the filled areas, but they do look like they belong to the correct net (e.g.: when you select the net).

I've made a "rounded corner filled area" joining four partly overlapping rectangles and four circles (see below) but it's probably a bad idea.

That's beyond me, let's see if @max has any further ideas.

max

To connect the GND you first connect in the schematic the power symbol GND to the two pins like so:
Then you need to decrease the Copper to edge clearance in the Board Setup
Now assign the GND Net to the copper and you can route to it.

max

You can make your project much nicer if you ad net labels to your schematic, then the nets will have clear naming:

insultcomicdog

max

Thanks so much for you help! I added ground power symbols in my schematic and decreased edge clearance.

When I try to assign the GND net to that ground plane I can only assign one pin either Pad 1 or Pad 32, not BOTH at the same time.

I was able to still about to route both pins out from connector, but only assume one trace is actually connected to the GND plane?

I added net labels to schematic, but I'm not sure why still my vias / and traces all still are labeled as unconnected.

I ran DRC with only these errors remaining.

For my actual design I plan to use an imported DXF or SVG for touch pads. I'm just working through this tutorial example to understand the workflow and learning KiCad.

Here's my updated file:

customeflextrillsensor.zip

300kB

giuliomoro

The "unconnected" is part of the net name .

When you update the schematic you should press the "Update PCB from schematic" button
in the PCB editor to update the name of the nets. Then you will see that GND is actually called GND and that the same signal goes to pins 1 and 32.

What Max was suggesting above

You can make your project much nicer if you ad net labels to your schematic, then the nets will have clear naming:

was exactly to give names to the nets in the schematic in order to have prettier names in the PCB.

As you've done that in the schematic already, once you press "Update PCB from schematic", it will look like this:

insultcomicdog

giuliomoro

Thank you! Update pcb from schematic fixed the names for my traces and GND issues for my ground plane.

The only error I have left is this from DRC:

max

Looks like you are missing a via at each end of the GND trace to connect from one side to the other.

giuliomoro

regarding the DRC error, it seems that there's a shape on Edge.Cuts on the footprint and I don't know whether you can merge that with the one on the PCB. This results in two conflicting shapes on edge.cuts. You can fix it by opening the footprint in the footprint editor and moving stuff from Edge.Cuts to another layer (e.g.: F.Silkscreen). Then the DRC should pass

insultcomicdog

giuliomoro @max

I added the vias to the GND plane. When I drew the outline on the Edge.Cuts layer, I drew lines over the connector foot print. I deleted the lines overlapping the foot print and all my DRC errors are gone.

I only have these 4 warnings now:

Do I need to address these warnings before sending files to production house?

giuliomoro

did you paste the wrong image? That one has two errors , not four warnings

insultcomicdog

giuliomoro You're fast. Refresh page I edited and reposted correct screen shot.

max

You may ignore those warnings. Just the silkscreen is clipped by the board edge.

insultcomicdog

max

OSH Park has temporarily suspended fabricating flex pcbs.

I'm trying to submit gerbers to JLCPCB which only supports .12 mm pcb thickness for flex pcbs. With added .2mm thickener the total thickness is .32 mm.

Will that fit the connector?

They also have .225 and .25 options for Polyimide thickness.

giuliomoro

we recommend 0.30mm±0.05mm, so 0.12mm + 0.2mm will be fine

PCBWay does 0.16mm + 0.2mm stiffner and that also has worked well for us in the past.