I opened your PCB in KiCad-nightly V6.0.0-rc1 and it does show this artifact in Pcbnew itself:
KiCad-nightly V6.0.0-rc1 also can not render the PCB properly in the 3D viewer unless I delete this circle from the PCB.
I’m quite impressed with the VNH7070AS. And 15A 40V H-bridge in such a small package. It does seem overkill for an N20 motor though. Maybe a cheaper driver such as the Allegro A4950 is good enough?
Your PCB still shows some ratsnest lines and has unconnected items, and these are real faults. One of them is on the south side of the PCB:
Note here that pad 2 of R28 is connected to a small part of a copper zone, but not connected to the rest of the GND plane.
The same for the North-West area of your PCB.
The encircled orange part is not connected to the rest of your GND plane.
KiCad-nightly V6.0.0-rc1 also has an improved DRC, and it flags a lot of “Track has unconnected end” violations. Most of these are not important, but some do require attention. Below for example, you’ve drawn two via’s to increase current handling, but one of the via’s is unused.
There are also some more examples (at least 2) of this in the +3V3 net.
In a general sense, you have copper zones connected to GND on both the top and bottom of the PCB, but these do not combine into a proper GND plane. Both of them are cut into little pieces by copper tracks.
When you are designing a PCB, one of your goal should always be to have one uninterrupted GND plane. You should bring as much tracks as possible to the top layer, even if it means using more via’s on your PCB.
You have drawn C4 and C5 as 270uF capacitors and used 0805 sized footprints for them. This would not work. These are probably electrolytic capacitors. You should also put them closer to the VNH7070AS IC’s (for the ceramic decoupling caps C6 and C7 this is even more important). I suggest to move the testpoints TP1 through TP6 further away from the IC’s, and put the decoupling capacitors in those locations, and as close to those IC’s as possible.
I also suggest to add 100nF decopuling capacitors to both the modules U8 and U5. Put these capacitors close to the power pins (Pin1 1 for both U8 and U5).
Also, ceramic SMT resistors and capacitors are quite fragile, and your PCB is likely to see a lot of abuse. These parts can break if the PCB gets bent or twisted. Resistors tend to ail open when they break, but capacitors often create a short circuit when they fail. One way to fix this is to solder them vertically on the PCB, and then solder a short wire to the other pad. This looks extremely ugly and unprofessional, but the short wire can bend a bit and this prevents your parts from breaking when the PCB gets bent or twisted. A better way is probably to use old fashioned THT parts in this project. Some PCB manufacturers also make thicker PCB’s for a small extra cost.