Strange ERC-Warning

Schematic
1

Hello all,
I have a Problem with a strange ERC warning. It says:
Warning;Symbol pin or wire end off connection grid
My Problem is, that I imported this schematic from another KiCAD V7 into this schematic which is a V8 schematic. The strange thing is:

  • List item

the warnings did not appear in V7 (I think it was V7.03
all wires are connected (I checked all warnings manually).
the warnings occur on wires that are drawn in one line but with angles
the warning is only set on the angles and junction-points, but not on the connection to a symbol
the align items to grid doesn’t help

2

Excuse me, fingertrouble. I didn’t want to send the incomplete message.One Item is missing:
I tried to delete a wire with the warning and drew the wire again and got the same warning.
Regards
Norbert

3

Items being “off grid” is unfortunately a relatively serious problem with KiCad, that nearly everybody will bump into at some point while working with KiCad.

In KiCad all pins of all symbols should be on a 50mil (1.27mm) grid. KiCad uses the active points of pins and the endpoints of wires to build the netlist. In later KiCad versions some snapping has been added to the schematic editor, but it’s still not best practice to rely on that. to make life easier for yourself it’s recommended to use a 50mil grid in the schematic editor (25mil or 20mil may also work) but not finer or coarser.

This “problem” has always existed in KiCad, but in later versions there are now both better tools to check it, and tools to fix it. If it is caused by the location of the symbol, then the simplest way to fix it is:

  1. Set the grid to 50 mils.
  2. Select everything in the schematic, then a right click and select Align elements to Grid from the popup menu. KiCad has an extra quirck here. In some cases wires from different nets may end up at the same location and then cause shorts. So check for that. For example by updating the PCB, and running DRC to verify connectivity of the netlist.

It’s also possible that your older symbol (especially when self drawn or from other sources) has one or more of it’s pin off grid. In that case, modify the symbol in the symbol editor. The symbol editor also has: Symbol Editor / Inspect / Symbol Checker and this also checks for off-grid pins.

4

My Problem is, that I imported this schematic from another KiCAD V7 into this schematic which is a V8 schematic.

There was a change in the working principle for this specific ERC-check:

  • v7: the “wires/pins are located on/off grid” check used the current set grid value (set from the grid menu)
  • v8: the “wires/pins are located on/off grid” check uses a dedicated value in Schematic Setup–>General–>Formatting

So make sure you have a appropriate value in the schematic setup.

5

@paulvdh, @mf_ibfeew
Thanks for your tips. Yesterday evening I found out that I had to change the formatting in the setup menu. I had to change the grid on/off from 50mil to 25mil and the warnings were gone. But it still looks strange to me because of three reasons:
Some of the symbols had this warning on there pins and some not.
After I redrew one of the wires the warning was still there
The warning appeared at every angle of the wires, even if they were drawn in one peace without any break. Obviousely KiCAD devides the wire into parts even if the angles are generated automatically by KiCAD.

But now I know what I have to do and I can live with it.

Thanks for your help.

Regards
Norbert

6

That means you probably also had a 25mil grid in KiCad V7. You can either keep doing that, or set the grid to 50mil and then do the Align elements to Grid thing I mentioned above.