What does 'Rect on B.Cu' mean?

I keep getting the above error in relation to this part


Here is the exact error message:-


I’ve checked and there does not appear to be anything on the back copper side that is wrong and the board looks clean in the 3D viewer.

I changed the part (and others that I had made) so that both pads on the part are now numbered 1 (previously 1 and 2).


rect == rectangle
Note that simple graphic shapes have a “no net” property and can’t be assigned to a net. So a graphic shape produces always a clearance conflict with a track. (exceptions are custom shaped pads which are build from graphic shapes, and maybe nettie pads).

Note also that you should always mention the used kicad version. I have assumed you work with v7. The answer above is not 100% true anymore in upcoming v8.

Thanks - I am using V7.

I’m trying to understand how this works if I made a component. Here is the symbol I made


When I draw the schematic, I call up the footprint symbol so was expecting there to be a 1:1 match.


Here is the symbol I use for a test point:
It is found in the standard KiCad symbol library under the name “TestPoint”

The associated footprint I use can be found in the standard KiCad footprint library under the name “TestPoint_Bridge_Pitch2.0mm_Drill0.7mm”

3D view shows the loop of wire as the installed component:

Assuming this is the desired result.

Additionally, if there is room, I put a second test point nearby connected to common/ground/return (whatever is appropriate) for the return path from the test probe.

1 Like

A schematic symbol has almost nothing to do with DRC errors in PCB–unless you did not map pins correctly.

You should be also looking at and sharing the footprint you used.

That’s a nice looking TP clip. If I place the schematic symbol on the circuit with the pins defined as (1,1) and then associate that with a footprint with pins defined as (1,1) surely that should work, assuming no other errors (I can’t see any)?

Here is the footprint

Here is the 3D rendering (front)

Rear View


. If I place the schematic symbol on the circuit with the pins defined as (1,1) and then associate that with a footprint with pins defined as (1,1) surely that should work

No, that will not work.
For all schematic symbol the restriction is “all pins must have different pinnumbers”. So it’s forbidden to have a symbol with two pins with pinnumber==1.
After creating/modifying a symbol always run the symnol editor–>Inspect–>Symbol Checker command. This will report such easy mistakes.

For symbols /footprints there is the rule: all pads with the same padnumber are connected together and connected to the pin (from the symbol) with the corresponding pinnumber. You can have multiple pads with same padnumber (as in “TestPoint_Bridge_Pitch2.0mm_Drill0.7mm” shown by the @tryitagain ), but only one pin with that pinnumber.

Look and examine the shown examples (symbol “testpoint”, footprint “TestPoint_Bridge_Pitch2.0mm_Drill0.7mm”). The symbol has only one pin, numbered as Pin==1. The footprint on the other hand has two pads, but both pads are also numbered as pad==1. In the resulting schematic/board both pads are connected together.

Maybe copy both (symbol+FP) in your own library, play with them, try to modify them and gain experience.

Thanks - that makes it clear :+1:

Copy the “Test Point” footprint into a personal library.
Open the Test point in that personal library in your Symbol Editor…
Add the graphic rectangle on the bottom layer to join the two pads, as you have done in the PCB editor.
Right click one of the pads in the symbol editor.
Select “Edit Pad as Graphic Shape”.
Select “Edit pad as Graphic Shape” again, to close the function.

Now you have a new footprint consisting of two pads connected with a graphic rectangle all in the one footprint, so DRC will not complain. :grinning:

1 Like

Fantastic - thank you!


1 Like