Sorry, but my reply to you is above, somehow directed to someone else… Not sure why that is? I am not sure if you can see that reply… Let me know.
I guess here you are drawing tracks on the pcb? I will have a look if I can get that to work…
The coarse segmentation issue exists in 5.1.x but is resolved in the development branch. Unfortunately, it required a file format change.
I’ll have a look at whether there is some partial fix we could implement in 5.1.3 to improve this situation…
3 Likes
Hi @Seth_h I managed to move the tracks editing with a text editor the kicad_pcb file to B.Cu, but this is a bit tricky…
btw how is doing your work on curved tracks for v6? Any news?
1 Like
Somehow I get the impression that OSH Park does not see these tracks on the B.Cu layer. Still looking into it… 
Your arcs are not on copper right now. They are on Eco1.User.
You can move them to copper or select the arc with one of the pads, right-click and choose “Create Pad from Selected Shapes”
Progress generally visible here[1]. I try to push after each editing session. I’ve been a bit slow as I’ve been dividing time with launching a KiCad for business support venture. There is an amazing amount of paperwork involved. 
But it is coming along. Both should be out in July.
[1] https://code.launchpad.net/~sethh/kicad/+git/kicad/+ref/curved_tracks
1 Like
I’ve been experimenting a bit, and I’m wondering what I’ve put myself into 
David has certainly put a lot of time and effort in this thing and the complications of this being avery weird board (compared to normal PCB’s), and current limitations in KiCad make this a very bad board for beginners to get to know KiCad.
When using the “create pads from Selected Shapes” as I originally suggested. the created pad does indeed look ugly, and with big straight pieces, as in the red track in this creenshot from Pcbnew:
However, this is just a drawing artifact, beause if you select the custom pad in the Footprint Editor, and look at it’s properties, and then the tab “Custom Shape Primitives”, you can see they are clearly defined as arc segments:
I’ve also made gerber files of this connector, and in the gerbers there are more segments, with shallower angles, ie, they look more like arc’s, but still have visible segmentation. If this board gets manufactured, it will very likely be OK in this regard.
Another complication I see is that there are very small clearances.
In the Flex connector at the bottom, the clearances between the connector tracks are not uniform, and some are as low as 83um.
Also on other places the clearances are not uniform.
In the center I see 2 circles used as references, but I do not know which is which.
It all resembles hand drawing and guesstimating, and that is not a good sign for aboard with such small tolerances.
With such small clearances you clearly want a reliable DRC to make sure the clearances are met. Which is even more important because of the segmentation i the arcs, which distorts their true shape.
A test upload I did at Oshpark looks like it works if I add a simple rectangular board outline, and move the tracks to a copper layer.
Simply moving the tracks to copper as Setth_h suggests also is not a good idea.
It creates graphical items on a copper layer, and currently KiCad has no DRC for them, and therefore it will not flag your low clearances.
1 Like
In my post #20 where I suggested to build this from an array of lots of short segments may be the best option if it’s drawn completely in KiCad, because all the pieces are “normal tracks” and can therefore be checked by DRC.
And yes, I did that experiment directly in Pcbnew by simply drawing some unconnected tracks and dragging enpoints to snap on each other…
1 Like
Thank you very much for that! I will have to go back to the drawing board! And it explains that OSh Park still did not see the footprint.
Btw the circles in the middle where indeed different points the different circles where drawn from. The tolerance of the board itself would have been fine as the cutout was as required and also the connectors where in the right place. But the traces have to have some durability as it is dynamic and moves regularly.
Thanks again for the assistance!
but have you uploaded the board or the gerbers?
and have you included also the pcb edge?
would you mind to share the board with the board edge?
1 Like
Those circles are 0.55mm apart, which is more than your track with or clearance.
A quick check of the biggest arc’s of the track (on the top) reveals that they are not concentric, and their centers do not coincide with either of those center marks ???
etc.
Other arc’s are also drawn with different center points all close to each other. Is it really important to keep those centers 0.55mm apart?
If I were to draw this flex PCB I would choose (0,0) as the center of all the arcs.
Also, I’m curious how good it will work to draw the tracks in the way I suggested in #20, but it I would like to put them in the right spot at the same time.
Can you zip the whole project and upload it as a single file?
Having a working board outline to work with will give more confidence that I’m going in the right direction.
Also, Now I see the outer tracks with a width of 0.3mm, and the inner 2 with a width of 1mm, (and some variable clearance).
Can you give more accurate numbers for these measurements?
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.