Greyed out Options

Using 5.02 and am trying to learn from zero. Searched google trying to find out why edge cuts are greyed out in the footprint editor but not in PCBNew ? Obviously not a programmer but trying to follow along with the most recent tutorials I can find, with relevant content, and running into several layers in the editor being greyed out.

Wondering if that’s why I’m running into these issue with downloaded footprints from a SnapEDA ?

Might not be related but it seems odd to me that the edge options are greyed out in the editor and when viewing the footprint in 3D, the normal green PCB outline is invisible. Is there any plan to turn these greyed out features back on ? There are zero answers on this subject other than editing in a text editor, which honestly defeats the purpose of a 3D program package all together.

First: Please start by stating your KiCad version correctly.
There is no KiCad V5.02. V5.1 is expected within a few weeks.
So I’ll assume you have one of the KiCAd V5.0.2 versions.

Next: Your screenshot is very vague, so I’m mostly guessing what you have done.
Why do you think those layers should be enabled in the Footprint Editor?

Edge.Cuts is rarely usefull in the Footprint editor. Some components are designed to be mounted in a cutout in the PCB (for example some low-profile USB connectors).

The 3D viewer is a bit finicky when it comes to board outlines. On my Linux box it tends to not start or crash if the board outline is not properly defined.

If you want to experiment with the 3D viewer as a beginner, then start with a PCB with a fully closed & valid outline.
Have you installed Kicad-demos? There are some fully designed boards in there to experiment with.

When the 3D viewer is started from the Footprint Editor it usually shows a small dummy PCB with the size of (presumedly) the Couryard layer, or the smallest box that fits the component outline.
You are probably looking at a footprint of a component without a 3D model, or have turned it off in the settings of the 3D viewer.

The 3D viewer can turn on / off some settings:

3D-Viewer / Preferences / Display Options
And there are other menu’s also greatly influence what it looks like.

Have a look at the board from this thread:
When you experiment with the settings you should be able to have something similar to the screenshotr there on your own screen.

Yes the edge cuts layer is disabled in the footprint editor. I never got a clear answer from the devs why this is the case. I think it is mostly because they did not want to invest the time to check what can go wrong when enabling this layer shortly before the v5 release (The wishlist bug requesting edge cuts layers in footprints heated up shortly before the feature freeze as i got interested in this topic at that point in time.)

We at least got it to the point where footprints with edge cuts drawings are displayed correctly in the editor (In the past drawings on that layer got moved to a different layer when opening a footprint.)

Meaning right now the best option would be to draw on some otherwise unused layer and move the drawing to the edge cuts layer using a text editor. dwgs.user or one of the eco layers come to mind. Alternatively you can also use B.Fab as one can draw directly on that layer in the footprint editor.

For reference the wishlist bug:

1 Like

The official stable release is 5.0.2 as stated on the main website. That’s the version I’m using.

That dummy PCB displayed is what I’m talking about. Not sure how that screen shot is vague, as it clearly shows the dummy PCB is missing. All you can see are the pads and through holes. I have changed no settings yet, other footprints display fine.

SnapEDA doesn’t export to KiCad very well. Here it is with extra layers hidden.

It’s not good to define slot holes as board outlines inside footprint files. SnapEDA has exported courtyard and component outlines to extra layers, therefore they aren’t visible here. Edge.Cuts has text, that should never be done (board manufacturers don’t like it). The actual edge line is just a suggestion and it would be better to put it in an extra layer.

In my experience SnapEDA files can be used as a base but not as-is.

Here’s the 3d view after Edge.Cuts is removed:

I agree with Rene that the software should allow Edge.Cut in the footprint editor, but still personally I’m not sure about the usefulness of such in most cases. I draw the suggested outline in an extra layer and position the footprint accordingly along the board outline in the board editor. Normal USB Type C or other connectors rarely need complex board edge, there’s only a straight line, and even that is a suggestion. Exact position depends on chassis etc.


There are some components that simply need that layer defined in the footprint
Examples are:

  • components that have large features that require a cutout (Holes larger than 6mm or so are most likely not supported by your fab. cutouts with relatively sharp corners can not be made any other way, …)
  • edge connectors that use the shape of the pcb plus pads as the connection part like for example a typical PC card for pci or pci-express or even the ram slots.)

You are however correct that the footprint at hand does not need that layer as there are better alternatives available (oval holes)

Now I also remember that if Edge.Cuts was enabled footprints could be used as outline templates, although it would not be without problems for other reasons.

Some people might also use edge lines for simple “oval” holes because their manufacture may like it better (I have understood that not all manufacturers accept slots in drill files).

In any case the software shouldn’t restrict people doing what they want if there are good reasons to do it.

1 Like

eelik, how did you fix the footprint ? Text editor or in the footprint editor ?

In the footprint editor. Turn off other layers and the Edge.Cuts is still visible. Then you can easily select and delete items there.

1 Like

You might have a negative too much here or i am too tired. But i agree that the software should allow users to do what they want. Especially if there are valid reasons to do it the way they want. (All this handwaving in the bugreport about wanting a proper implementation is not really beneficial in this case as disallowing this layer really limits kicads functionality unnecessarily.)

1 Like

In the Footprint editor you can click on an item to select it, press “e” for edit, and then change it to another layer.

Here is an example of “Low profile” USB connectors that need a cutout which would be nice to have in the Footprint itself, but a “suggestion” on another layer is also usable.

Another example are card edge connectors which often have a precicely defined edges and cutouts.
A potential problem though is that KiCad needs an exact continuous polygon on Edge.Cuts. This is easy to realise when all line segments are on the same grid, but when a Footprint adds some lines to Edge.Cuts this does not work anymore.

1 Like

While browsing KiCad’s own library I stumbled into a foot print that already looks a lot like the SnapEDA Footprint.


1 Like

Thank you for the help. That seemed to work.

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