No-connect symbols cannot eliminate error


I put no-connect symbols to eliminate the no-connect errors. But, It doesn’t make sense.
I don’t know why. I try everything, but it still cannot work.
Can you help me?


You seem to have a grid problem. You have used several grid pitch values, maybe two, and one of them is so small that things are a bit off. The same problem is in the wire/wire connections and wire/pin connections.

Symbol pins should always use 50 mil or larger grid value when symbols are created. You should also use 50 mil grid for the schematic. That way it’s possible to connect pins, wires etc. properly.

Now you should redraw some parts of the schematic, using 50 mil grid.

1 Like

Hi @Gaoshen39568652, after @eelik’s comment i also want to advice to pay attention when moving and draging symbols or selected elements, or paste a selection. This is also a moment that might cause grid misalignment.

1 Like

That explanation makes sense sometimes. In this case for example the no-connect marks aren’t systematically off grid but in different relative locations, so there’s probably a very small pitch value for the grid used here.

Just for your information: this is a long standing problem in KiCad. The situation is a bit better in the unstable development version 5.99 where it’s possible to snap to items and there’s also a context menu item “Align Elements to Grid” for selected items which could fix this at once. But still it’s best to use only one and the same grid always.

1 Like

I don’t understand why the option to change schematic grid is made so easy to (ab)use
There are very few good reasons to every change from the default and beginners keep making this mistake

I’m far from a power user. In my case forcing pins to 50 and making everything else ‘don’t care’ would work for me. I simply find 50 too course for the text portions. That’s the only reason I need to change.


When I check the components’ pins, they look like normal, I don’t know why.
Another question is when the grid intensity is 50 mm, it is hard to put the wire on the pins.
Screenshot from 2021-10-29 11-14-06

X and Y position of that pin tell that it’s in the standard grid, so that should be OK, if other pins are also in multiples of 50 mils.

The problem is then the schematic editor grid. Once you have placed some items using a “wrong” grid which is incompatible with 50 mil grid, it may be difficult to fix the problem. Basically you have to switch back to 50 mil grid and move the off-grid items. Because they seem to be in a small pitched grid and not placed uniformly compared to the 50 mil grid, you have to move them one by one. That way they snap to the 50 mil grid. But in v5.1 you can’t select several items to snap them back to the 50 mil grid.

At my beginning with KiCad I also changed grid after inserting each element to place its reference and value texts as I wanted them and than back to place following element and so on. I worked that way until someone told me about CTRL+SHIFT combination for placing texts. Since then I never change grid at schematic.


Yes, I am using kicad 5.1.11. How to snap them back to 50 mil grid?
Do i need to change a lower version kicad? do you have a recommendation?

Change the schematic grid to 50 mil if it’s not already. Then move one item normally: hover over it, press M and drag with mouse. If the item was off-grid it first snaps to the 50 mil grid.

Unfortunately this is quite much work for you because you have so many off-grid items and the no-connect items overlap with the symbol, so you have to clarify selection for every item. To be honest it may be easier to just start from scratch for the part of the schematic which has off-grid items.

On the other hand, if you are just starting with KiCad and the design isn’t critical, you could consider switching to 5.99. It’s still under development and has bugs but it’s relatively stable. Many users have used it successfully without problems. It will be released withing couple of months anyway as v6.0.

As I said, in 5.99 there’s a function to align several selected items to the current grid at once. The editing paradigm in 5.99 schematic editor is different from 5.1 and you have to learn it soon in any case because v6 will become the recommended stable version.

Remember that the same problem is visible in several other places, for example


You can see small squares in all locations that eelik encircled. Those sqares (and circles for symbol pins) indicate that that KiCad does not recognize the connection.

KiCad relies on perfect matches of the coordinates of the endpoints, and that only works when the grid is set up properly.
The current workaround is to simply never set the grid to a value below 50. A grid of 25 is probably also coarse enough to be able to make connections easily.

Texts and such can be placed off grid by depressing both [Ctrl + Shift] while dragging them.

I once read something on gitlab about a proposal to use different grid sizes for “electric stuff” (symbols, wires, etc) and other things such as texts.

1 Like

Where to download version5.99?

Do not use the old KiCad website. It’s likely to have (or get) malware at some indeterminate tie.

Like Paul said. It’s also called “nightly builds”.

Thank you very much for all!

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