How fix the wire connection problem [solved]

Schematic
1

Hi everybody
I am facing wire connection problem with both built in library components custom made too.
Thanks

1040Ă—1857 888 KB

2

Right click in an empty place in the schematic >> Grid select >> 1.27mm …

2 Likes
3

Something is mixed up in your grid. Your components should be on the same grid pitch as the schematic.

Check this video on minute 36 the same thing happens there.
Correction: IT’S MINUTE 36

3 Likes
4

Make sure you run DRC checks on your custom components in the library editor. All pins should be on the 50mil grid to avoid these connecting problems

5

Solved thanks
:blush:

6

4 posts were split to a new topic: How to create footprint

7

A post was split to a new topic: Schematic wire connection

8

Had the same exact problem. Setting grid to 1.27mm resolved it. Anyone care to explain what happened or why that fixed it?

9

KiCad does not snap to connections.

For connections it depends on coordinates to match exactly (on it’s 1mill = 0.0254mm) internal coordinates. It is possible to make connections on this resolution when you zoom in a lot, but it is still very cumbersome.

All of KiCad’s symbol libraries are defined with all pins on a 100mil grid (See KLC and when you also keep the grid in the schematic on a size compatible with that, then the coordinates of the pin attachment points align with the endpoints of the wires easily. 50mil works good in practice, when you set the grid to smaller then 25mil, it becomes increasingly more difficult to align elements properly. It’s one of those things that are not exactly ideal in KiCad, but it’s “good enough”, and there are still a lot of issues that are either more pressing, or more interesting to fix and/or extend KiCad with.

If you’ve gotten yourself into this situation you can “fix” it in KiCad V6 by:

  1. Set the grid to 50mil.
  2. Selecting everything in the schematic.
  3. Right click and select “Align Elements to Grid” from the popup menu.

image
image811Ă—718 67.8 KB

1 Like
10

@stormbytes

Just to further comment on Paulvdh’s post:
When working with the schematic, it is best practice to exclusively use 50mil (1.27mm) when placing or moving wires, buses and all symbols.
Use other grids, where required, for adjusting text and image locations.

2 Likes
11

Understood. Thanks for the tip!

1 Like
12

Just leave the grid at 50 mil and press CTRL before moving text, it allows free placement and you don’t have to revert your grid

3 Likes
13

Thank you. I only use the Eeschema module for drawing. Just tried CTRL and is ideal for my usage of positioning in various boxes.

14