I’ve been using KiCad for a few years now. In my current project using 8.0.5, I can’t seem to correctly connect component pins with wires and labels anymore, due to how grid placement works.
This post is about the following behaviour: I have reset the grid settings to default, placed an inverter component, snapped two labels on either side (the labels visually snapped to the pins). I then enabled showing the grid and zoomed in - there is no visual indication whatsoever that the connections are off-grid at this point. I then run the Rules Checker and find an off-grid warning and a Label not connected error for one of the labels.
Then when I click on the component or the labels and press ‘m’ for move, they slightly snap to a neighbouring position, obviously on some grid. But each one seems to snap to a different grid, because I am not able to join all three (inverter component, input label, and output label) to form a proper connection without warning messages.
I’ve had this problem in past releases, and somehow worked around it (to be honest, I think I simply disabled these Rules Checker warnings). I understand that this must have to do with me changing the grid size (perhaps inadvertently). But I would assume that selecting all three components and right-clicking “align to grid” would sanitise placement of the selected items.
What would be a good method to recover my schematics to working order (I can snap to grid all I want, but it still won’t connect), and what are reliable indicators for when I am placing “outside” of connection points. Surely, no designer will ever intentionally place any sort of component where it won’t be able to connect to other components, and yet it can happen so easily?
I’m very pleased with KiCad on the whole, and I’d like to thank everybody for your forum input!
I am not sure what the cause of your problem is, but my first guess is that the symbols you use are themselves not designed on a 50mil grid. Does this only happen with symbols you design yourself, or also with symbols from KiCad’s default libraries?
You can verify problems with pins in symbols by first loading it in the symbol editor. This can be done directly from the schematic by hovering over it and pressing [Ctrl + e] and then: Symbol Editor / Inspect / Symbol Checker, which reports off-grid pins:
And what do you consider a “default” grid? I am not aware of a “reset to default” function, except by deleting files in the configuration directory. KiCad V8 also has a “grid override” system, in which grids for different item types can be set at different resolutions.
Thank you for replying! The component I placed was the 74HC04 out of the KiCad library, so not a custom part. Just out of curiosity, I’ve checked the part as per your suggestion, and there were no off-grid pin warnings.
The “default” grid option I mentioned was the one in menu Settings/Schematic Editor/Grids/Reset Grids to default button, which I pressed to see if that would help fix my problem, which it didn’t.
I’ve now deleted my KiCad folder (macOS user) from the Applications folder, and re-installed it completely. I then created a new project (not re-opening my previous one), and recreated my dummy project with the HC04 inverter. I am still getting the off-grid warnings and not-connected error. Does re-installing the application not revert any and all grid-settings?
Thank you again!
If you create a box selection covering the inverter and labels in your dummy project; then right mouse select “Align items to grid”, do you see any shift in the labels or inverter?
I had to search a bit to find the grid reset button. I’d had to translate “settings” (as you wrote) to “Preferences / Preferences” (as it’s called on my installation of KiCad. I always use the exact same words when using “path names” through menu’s. It makes it easier to find things. (Especially for people having other languages).
No. that will not help. Re-instaling the same software to get different results only works on windoze.
I don’t use the fruit OS, so I do not know what this is:
I’ve now deleted my KiCad folder (macOS user) from the Applications folder, and re-installed it completely.
But resetting the grid as you did should be sufficient.
The “Align items to grid” is also unlikely to work, as on a freshly created schematic with default settings, nothing should be off grid in the first place.
I do remember a recent bug with connection problems, and KiCad suddenly not recognizing connections even though no coordinates in a schematic had been changed, but details are fuzzy.
@jmk, thank you! I’ve box selected the inverter and labels, then applied “Align items…”. The components shifted, but still gave warnings/errors on Rules Checker…
Thank you @paulvdh for actually listing the path to preferences. I had tried finding it, but was looking for ~/Library/Kicad… instead of ~/Library/Preferences.
This helped me to at least reset the grid-mess I must have created at some point in my KiCad installation.
If anyone has this problem of somehow corrupted grid settings on a Mac, I solved it by deleting the file: /Users/michael/Library/Preferences/kicad/8.0/eeschema.json
By “solve” I mean, that I can now right-click on any component, and “Align items to grid” will put the items selected on the same grid, so that they connect.
I still need to do this manually for dozens of components now. It would be nice if KiCad would categorically not allow any sort of off-grid placement. When this happens (possibly inadvertently due to a clumsy key-chord altering the grid size), it is just a needless, immense loss of time and productivity. I know there have been posts on here along this theme, so I don’t want to belabour the point.
I really appreciate the help you’ve provided! : )
Draw a big selection box around the whole schematic.
Do the Align Elements to grid thing for a whole schematic sheet.
KiCad is (slowly) getting getting more strict here. For example when in the symbol editor in KiCad V8, you get a warning message whenever a pin is placed off t 50mil grid. But I do tend to agree with you. This is not an issue at all for people who know KiCad, but it is a very common beginners mistake, and this makes beginners less happy with KiCad, and thus it enlarges the chance they go on to use some other program. and that’s a missed chance for KiCad.
Thank you @davidsrsb, that sounds like a helpful additional check! @jmk_and_paulvdh: The “Align elements to grid” works for me now, even when I select multiple components - my installation must have really had some weird grid settings (possibly combinations that were only possible in earlier versions?), as that didn’t work before.
I have sometimes noticed symbols / pins ending up unaligned to the electrical connection grid, but have never managed to make it repeatable to fix. Can happen with hierarchical sheets / pins too.
