I try to route a rubber dome golden finger in Kicad 5.1.10, but it appear a message:
Anyone can help me to solve this problem?
Here is my PCB file.
example PCB.kicad_pcb (76.6 KB)
The error message is a bit confusing.
The actual error is that you use graphic items on a copper layer in your key footprint. KiCad does not recognize graphic items as copper tracks.
The way to fix this, is to add the graphic items to the pad. Do this with:
- Open your key footprint in the footprint editor.
- Select a pad and all connected graphics (Arc’s, horizontal lines)
- Right click and select "Create pad from selected Shapes from the popup menu.
- Repeat for the other connection of your footprint.
- Save, and then update your PCB with the modified footprints.
Also:
The polygon on F.Mask is a bit unusual.
First it complains about “Self Intersecting Polygons are not allowed” which is caused by two endpoints just right from the top having the same coordinate.
The best way to draw such a shape is to use an “aperture pad”.
First add a pad, then modify it’s properties to look like this:
*
Hi Paulvdh,
Thanks for your reply.
I try to do this, but an error appeared also:
so how to add a small anchor?
Thanks
You have to make a selection that includes a pad to make a custom pad out of it, and select all graphics that you want to turn into a custom pad at the same time like in the screenshot below. Note that the pad number is visible, and that pad is part of the selection.
While making a (complex) selection there is a differnce between dragging from left to right, or from right to left.
While holding the shift key individual items can be toggled into and out of the selection.
Also note that I unselected the F.Fab and F.Mask layers in the Layers Manger, so stuff on those layers do not distract (and also can not get selected) during editing.
Hi Paulvdh,
Thanks very much for your reply, now it’s very clear for me.
But for this issue, I have 2 suggestions here:
- The error indicator is not clear for me, maybe for many other people also. I don’t know what’s the meaning of ‘Cannot start rounting inside a keepout area or board outline’, and I also don’t know add an anchor point position if you don’t tell me to add a pad together with graphics, it’s great if Kicad has a much clear error idication in the program or in the manual in the future version.
- I have found a great footprint wizard to generate the button automaticly:
https://gist.github.com/mikerodrigues/fc8552d54756699811d05f1b80893cc9
And it’s published with the GPL liciense, could Kicad inlucde this wizard in the release package officially in the futhure?
Thanks
Sometimes UI strings are problematic, and in this case understanding it requires knowing something about KiCad which isn’t necessarily obvious to non-experienced users. “Board outline” should be obvious: you can’t draw a track which touches the, well, how could I say it to be more clear… board outline. And the reason should be obvious, too, if you understand what tracks are and what’s the board outline. You should never design a layout where a track is cut off because it’s not wholly inside the board.
A “keepout” is an area where certain items are kept out. In v5.99/6 it’s called “rule area” but the idea is the same:
Naturally you can’t start a track there. V5.99 gives a less intrusive and more exact message in the infobar:
FYI, in v5.99 the procedure to create custom pads has also changed. You select a normal round or rectangle pad and use context menu -> Edit Pad as Graphic Shapes, then draw overlapping graphic shapes which touch the pad.
Euhm…
xzf16 did not have a problem with the board outline.
xfz16 did not use any keepout area’s.
xfz16 is using KiCad V5.1.10, not the nightlies.
In this particular case the error message given by KiCad V5.1.10 was simply wrong and misleading.
I did open the pcb in KiCad-nightly V5.99 and it shows the correct error message “Cannot start routing from a graphic”:
Yes, I’m completely aware about what was and wasn’t done. Xfz16 expressed a feature enhancement wish which I told is solved in 5.99. It should solve the wrong/misleading message and make the messages more accurate in general. (One slightly annoying problem is still there: it says “from a graphic” for Edge.Cut lines, too, which IMO isn’t accurate enough because other than copper and Edge.Cut don’t prevent routing.)
If you wonder why I explained the message itself, it’s because of
I don’t know how much the original poster knows KiCad or EDA design, so I explained what these things mean in KiCad.
Hi Paulvdh,
That’s great that the Kicad 6 has improved the error indication.
I didn’t use v5.99 nightly build version because I used it in production enviorment for our business, and stable is very important for us. I am looking forward to V6.0 urgently and I am sure it will bring a lot of benifits for us.
No matter how, thanks for you kindly nice reply.
Hi Eelik,
Thanks for your kindly nice reply.
I am a freshmen for Kicad, I was used to use Altium designer before and I turned to Kicad in recent two monthes for our new project.
The approches of these 2 softwares are very different, so maybe I will post some other questions in the form in future, and sone of them will be very foolish in your side, please don’t mind.
Of course, I will try to solve them by serching them in The form before I post it.
No maater how, thank you very much again.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.