Warning Symbol pin or wire end off grid

Schematic
1

I have just upgraded to version 7.01, after having problems with 7.02. I now get tons of Warning: Symbol pin or wire end off grid. I have been reading that I can ignore this error, but how can I avoid it, and how can I fix a schematic that was created in version 6?

I have tried to build a test schematic from scratch, but if look like differen parts has different grid size, so what would be the best choise, if there is any?

Regards

Ulf H.

2

This is confusing and not possible to interpret… probably a translation problem.
You can upgrade from 7.0.1 to 7.0.2 or you can downgrade from 7.0.2 to 7.0.1.

Please explain your action and correct your statement. :slightly_smiling_face:

3

update problems aside (I also didn’t understand the order of your updates) the warning “Symbol pin or wire end off grid” was introduced (from v6–>v7 development) with the following background:

  • for connection between different nets and from nets to symbols the nets/symbol-pins must be on the exact same x/y-coordinate
  • all is well if the user uses a fixed grid (recommended: 0,05")
  • most connection-problems (especially for part-time users or newcomers) arise if a symbol (or individual symbol-pins) is not correctly aligned to that standard-grid - nets are not correctly connected to symbols
  • to help against these (often unintentially) unaligned nets/symbols the ERC-check “nets+symbols are on grid” was developed
  • this test checks:
    • if all nets start/end at a exact grid-position
    • if all symbol-pins are located on a exact grid-position
    • for this check the actual grid-size is used
  • v6 didn’t had this test - so it’s understandable that you get this warnings only with the v7-versions

So if this ERC-check shows many warnings there could be a connectivity problem. So you should:

  • examine the shown error-markers and decide: are the nets deliberately drawn or is there really a problem?
  • for this check the grid should be at the same setting as during net-drawing. If the grid is more coarse than during net-drawing than the nets are obviuosly located offgrid
  • if you often use varying grid-sizes (for instance to draw some nets on dense areas on small grid with very small clearance) - than this ERC-check may not suit your needs and you should turn it off
4

First of all, thank you for your answer. I am sorry for how i formulated the question, first part was not clear enough.

I first installed 7.02, but there were a lot of warnings when I started using it, and I found that these errors were repored as bugs, and that I could use verion 7.01 istead.

I would have reinstalled latest verion of 6 and waited for the bugfix, but alas my libraries was upgraded and I did not want to install all the parts I had downloaded once more.

When I start a project I have to decide what grid is the most favorable (I am not a very experinced user!) so do you have any sugestions about what would be a reasonable choise?

Best regards

Ulf

5

Use 0,05".
The standard kicad-libraries also use these 0,05" grid for all symbols. So this is the grid-value with the fewest problems.

advice:

  • change grid only for documentation purposes (value/reference-string, graphics / describing text-elements or so)
  • always switch back to 0,05" after using a finer grid
  • if you want to place these graphics/text try if you like the workflow with the “CTRL”-key as modifier: this switches off the grid-snapping for the current move-action. So grid-change could be completely avoided
  • if you already have some nets/symbols placed offgrid: select them (or select all on the schematic) → RMB-click–>context-menu–>align elements to grid
2 Likes
6

Thank you SO much! I’ll keep that in mind :grinning:

7

Was there a fix for this? My schematic has 999+ warnings for this. That’s a lot of connections to redo.

8

I got rid of most of those by pressing alt-2 which set my second grid size. 0.6350mm

1 Like
9

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