How to place a footprint by snapping to line end on Edge.Cut layer

[bgodk]

Hi,
KiCAD 6.0.0: I have imported a DXF file on the Edge.Cut layer with small 45 degres lines indicating the center location of a number of footprints. How can I place a footprint by snapping to e.g. the end of the 45 degre line on the Edge.Cut layer?

Is there a way/alternative to do that?

If this is not possible, I think it would be a candidate for a new feature.

Hints highly appreciated!

[mf_ibfeew]

read the discussion from yesterday: How to snap a footprint to reference geometry?

In short:

• snapping to outline (edge.cuts) is not possible
• having something other than the outline on edge.cuts is a bad idea anyway
• snapping works on line-ends (not tracks) on the copper-layer, so select your snapping-lines, use “Edit–>Edit Text and graphics properties” to change the layer of all the snapping-lines to copper
• set grid to some coarse value (will improve snapping behaviour)
• move the existing footprints towards your auxiliary-lines and try your luck with the snapping

If this is not possible, I think it would be a candidate for a new feature.

Snapping to any (on/off switchable) layer has already an entry on the gitlab-feature-wishlist.

[paulvdh]

@mf_ibfeew

snapping to outline (edge.cuts) is not possible

Not true.
While drawing a PCB outline, I often snap endpoints of lines and arcs to each other. This is the normal way of drawing a PCB outline.

@mf_ibfeew

snapping works on line-ends (not tracks) on the copper-layer,

Snapping to track ends also works. I made extensive use of this while re-creating a PCB form a set of Gerber files. (Gerber has no footprints, so I snapped the pads of new footprints to the endpoints of the tracks back imported from the gerbers. (A bit weird, but I can’t get it to work just now. Whenever I try to snap a pad of a footprint do a track end, KiCad snaps the center of the footprint to that track end, which is not what I want. Maybe I’m forgetting some setting, maybe it’s a bug.)

Snapping is a bit complicated. In fact, I’m not entirely sure when it does or does not work. In general, stuff related to copper layers does not snap to graphical stuff, and graphical stuff does not snap to copper items. There are also layer limitations. When you’re working on the front copper layer, it does not make sense to snap to items on the back copper layer. At least, for SMT parts. The pads of THT parts are present on all copper layers, and should therefore also use the snap points for those layers. (I think this works correctly, I have not verified this just now).

You can also change the snapping behavior with PCB Editor / Preferences /Preferences / PCB Editor / Editing Options / Magnetic Points. Magnetic points for Pads / Tracks / Graphics can be set individually.

On top of that, there is also the Selection Filter in the lower right corner of the PCB Editor. If items are not active there, they are just ignored.
To make it even more complicated, when you have “dimmed the inactive layers”, then snapping to them also does not work

If it all gets too complicated.
A workaround is to do it in two steps. First snap the grid origin to a point of interest, and then move the thing you wanted to snap to the grid origin. (This works best on some coarse grid).
Whenever KiCad found a snap point, it shows a small circle around the mouse cursor.

Just found some other weird thing. While changing the grid origin, (PCB Editor / Place / Grid Origin S), it seems to snap to all kind of internal geometry of pads.

I’m afraid this may all be more confusing then clarifying, but it’s the best I can do right now.

[bgodk]

The Place/Grid Origin S option actually makes the trick!! Maybe not the fastest method but it makes snapping to my Edge.Cut layer possible as you mention. Having the “place marks” in the Edge.Cut layer is maybe not a good idea, but i can replace it with one where the marks are removed.

Thank you for quick reply! You made my day!