Sometimes when creating a track through a VIA, KiCad creates a very small tracks (about 0.1mm) besides the normal tracks. I usually just delete these.
Do they serve any purpose? Should I leave them in place?
Is this a bug perhaps?? See image.
PCBnew puts tracks on the grid… the pads you are about to connect to (#23 I2C_SDA in that particular case) are NOT on that grid… the little piece of track now connects the grid-bound track via (green to it’s right) with the pad on the left.
If you run the editor in OpenGL mode the same applies as long as you don’t activate push&shove routing.
Deleting them is not advisable, as DRC might flag this as not connected anymore.
PS: switch your pads to non-fill mode to better see what you’re doing.
1 Like
These little track segments are created at other times as well, not just at vias. For instance when connecting to a pad with a track that is not aligned with the center of the pad. In the case above the via is not aligned with the center of the pad so the track that connects them has that little track segment in order to offset the track. Depending on the track posture the little segment will appear at the via end or the pad end.
They can be avoided in several ways, choosing a grid spacing that matches the pitch of the footprints, not always easy if you have footprints with a variety of pitches. Or start drawing the track from the pad that is not aligned with the grid. In the case above you could have started the track at the pad and avoided any misalignment resulting in small track segments.
Technically they are not required if the end of the track is sufficiently within the pad/via but deleting them can sometimes cause DRC to think the track and pad/via are not connected.
4 Likes
Thanks for clarifying and the tip! 
They also tend to get left behind when you delete a track. @Joan_Sparky suggestion of turning off fill makes it much easier to spot these runts