Invisible, unselectable rectangle breaks DRC

Layout
1

Hello,

I am working on the layout of a board. I have now found several instances in which as I am routing a new trace, this seems to collide with a rectangle. However, I cannot see, nor select it. Even trying to long-click to get the clarify selection menu, nothing that could be that rectangle comes up.

See below a detail of the board and the same detail as I try to route a trace. I set the router options to highlight collisions, so you can see the highlighted rectangle.

image
image1920Ă—2160 491 KB

As you can see, all layers are visible.

As an additional piece of information, I can say that the outline of this board comes from a OnShape project, exported as a R14 .dxf. Two graphics were included, one in the edge.cuts layer and the other in the F.fab layer, which contained additional component placement information.]

Finally, if I run DRC check after force-placing the trace that seems to break DRC, that doesn’t come up as an error.

I am working with KiCad 8.0.3 on MacOS.

Thank you in advance for your help.

2

Also make sure you have everything visible in the Objects tab of the Appearance panel.

On what layers are the
QFC …
C000 000
text and grey lines? They look suspicious. Make sure they’re not on the edge cuts layer as that would be interpreted by DRC as a border to avoid.

3

Is there a chance you started you design with a higher number of layers and reduced it on the way?

4

I see a copyright notice across the footprint centre. Is this an imported footprint, and if so, are those rectangles part of the import?

5

Hi all, thank you for taking the time to reply.

I think you were right. Now, by only showing the front copper layer and setting “Hidden text” to be visible in the Objects tab, I get some text to show up.

Screenshot 2024-07-18 at 13.23.52
Screenshot 2024-07-18 at 13.23.521920Ă—1080 239 KB

As you can see, there two pieces of text that seem to correspond to the two green rectangles in the previous picture. I showed the bottom copper layer for reference.

I think I know how that text ended up there. I previously wrote a script to automatically add an “MPN” field to all passives that would contain the generic code for passives that Eurocircuits expect. For example, in the picture you can see "GPC0402104’ for an 0402, 0.1uF capacitor. I think in the script I forgot to specify which layer should the text for the parameter be placed on, so it defaulted to F.Cu.

The solution now is to select each component that has this issue, set the parameter to visible so I can select it, edit the parameter so that I can move it to a different layer.

1 Like
6

Another way to fix it, is to first repair the library footprints, and then update the PCB with the new footprints.

  1. You only have to do it once for each footprint.
  2. Fixing the library improves your personal libraries.
  3. You can check whether the fix works in this current project.

Much better then just fixing it on the PCB.

7

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.