Hi. I’m making my first PCB with KiCad 7.
I am getting a “missing connection” error when doing the DRC for a pad that should be connected to GND.
I have examined the other topics where people had this issue, and I don’t think I have a ‘island’. The identical footprint right next to the one with the error, doe not give an error. So I’m confused. I attached a screenshot.
I tried to also attach the .pcb but it says “new users can’t upload attachments”
Thanks for any help.
Welcome @avsteele
Five more minutes of reading at least six more posts means you will be able to post attachments.
Read here.
Difficult to say without looking at the schematic. When your level has been increased can you post the zipped project
There are 2 unconnected tracks. If you zoom in and click on the green arrow you can see one small F.Cu copper track not connected.
You can either manually delete these or run Tools / Cleanup Tracks and Vias
There is a huge GND zone island from Q2 down to RN2. The other end of the ratline at J6 is joined to that island.
Hi @avsteele
The DRC is using pad 2 of J6 because it is the closest GND connection to the unconnected GND zone.
EDIT: DRC is telling you this with the remarks in the above box you first posted. It just takes a little practice to learn to interpret DRC 
Good spot on the ground island.
Ah that explains it why the disconnected pad is showing up as an error at J6.
Thanks guys for taking a look and the tips.
GMC: One question on the image you show. When I ran the cleanup tool I can see the arrows, but I couldn’t see those tracks unless I make the pads invisible or opaque, whereas they seem to show on yours. Is there a way to set the layer order?
There is probably is a way to see them from turning off various layers but I find it quicker to zoom right in, then on the DRC clck on the warning and it will take you to the spot with the issue. (Helps to have 2 monitors)
If you click on the green arrow near the tip you should see the unconnected track
I am surprised that at the picture in the first post there is no that ratline. I supposed that DRC error tells about connecting that pad to GND island but in such case I expected the ratline but it was not there.
Turning off Layers and Objects can often help with spotting stuff.
In this case, I turned off the bottom layer (in Layers) and the pads (in Objects) which easily shows the two stray pieces of track.
To turn layers and objects OFF and ON left mouse click on the “eye” beside the name of the object or layer.
EDIT: I could also have turned off Zones, Silk and F.Fab which would have only left tracks, to make spotting even easier.
Agree. Maybe the OP turned the ratline off?
That’s correct. While doing the layout early on I hid the GND net. That made interpreting the error more confusing.
In Protel I was always changing GND ratlines to blue and VCC to red and hiding the GND lines, but it was not possible in KiCad V4 and V5 so I learned to start work from doing the GND zone (at top and bottom) bigger then the whole PCB.
Pressing ‘b’ hides most of GND ratlines and you need not to remember to switch them back on close to end of design.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
