Parallel zigzag traces, and outline edge cut

I wanted to create a flex PCB, as it is a moving part I want to design a zigzag trace routing,
For understanding I have attached a pic of my incomplete design,
Can any one suggest me the better way or some trick to achive it easily. I do understand that using DXF file i can achive it but i am not good at other CAD software to generate it.

Is the board outline all 90-degree circular arcs? If so, you should be able to do this in KiCad’s router by setting a grid that is fine enough and setting the corner mode to 90-degree arcs

Setting the corner mode (with [Ctrl + /]) does work, but I think that working with graphical arcs works better in this case. In KiCad V8 net names can be assigned to graphical objects, and this makes them a part of a net.

I guess this method works:

  1. Set your grid to something suitable, such as the pitch you want between the tracks.
  2. (Optional, skip this in first attempt) Select everything on the Edge.Cuts layer and move it to another layer. I guess it gets in the way while drawing the arcs.
  3. Draw a bunch of arcs in the location you want them.
  4. Draw PCB tracks from pins to close to the arc’s. (KiCad won’t let you connect them yet, because net names don’t match).
  5. Draw a short horizontal track (not connected, both sides open).
  6. Make a copy of the track you just drew, and move one endpoint to the endpoint of an arc. The other end should overlap with an existing track. KiCad does not keep clearances while moving objects, and after the move it updates the net names of the overlapping objects. As a result, the netname of the arc (and the intermediate track) are both set to the net name of the existing track.
  7. Repeat step 6. to make some more connections.
  8. PCB Editor / Tools / Cleanup Tracks & Vias to merge the overlapping sections.

I experimented a bit, and this seems to work quite well, you can even work quicker by making a copy of a bunch of arcs you have already drawn, and copying / moving the “connecting tracks” can also be done as a block. In the screenshot below, I first drew the 6 arcs on the left side, connected them to the connector, then made a copy of all 6, moved that copy and used r to rotate the block while placing it at the new location. Using graphical arcs instead of PCB fillets is probably preferable. Graphical arcs keep their center. They do not get moved or manipulated by KiCad.

I also guess it’s good to experiment a bit with this workflow first, before you do the final artwork. While messin’ a bit around you can get a feel for what does and what does not work well, and when you do this with just two or three tracks, mistakes are quicker to correct.

1 Like