Is it possible to draw edge cuts by specifying corner X- and Y- coordinates?

Hallo everyone,

Does KiCad also allow drawing edge cuts by spcifying the X- and Y- coordinates of four corner points instead of clicking (at one board corner) and dragging the cursor with mouse around the board peripherie back to the starting corner?
If yes, where can one select this option, please?

Thanks for your support in advance
Best regards

Not directly but you can easily specify the start and end points of any line. Draw a line on edge cuts and then hover over it and press ‘e’. The ‘Line segment Properties’ dialogue will be presented and you can edit the start and end points of your line there.

One other useful trick is to set your grid to a multiple of your board size. e.g. You have a board 35mm by 45mm - set your grid to 5mm spacing and it is easy to draw an outline of the correct size. Subsequent lines you draw should also snap to the end points. Pressing Cmd constrains any lines to horizontal or vertical.

Screen Shot 2020-02-09 at 15.35.00

2 Likes

Thanks a lot, John_Patman,
Your first tip (i.e. hovering over the line and editing properties) worked fine.
Thanks for your help
Best regards

Another option is KiCommand, a plug-in I wrote for exactly this type of situation. Easy command line access to pcbnew. I’m working on a tutorial (search this forum for it) in which I teach KiCommand from the basics.

In the process, I’ve noticed some additional commands for manipulating or adding PCB elements, which i’ll Add over time.

As an example, adding an edge cut rectangle should go something like this:

Edge.Cut layernums l param 0,0,0,20,30,20,30,0,0,0 mm drawsegments

If you need help, there’s also a discussion thread available.

2 Likes

And a third option is to make use of the custom grid. Place the grid origin at your first coordinate and set the custom grid spacing to whatever you want the size of your board to be.

1 Like

How do you set the grid origin in pcbnew ?

The grid origin is set via the tool from the right toolbar or in the custom grid dialog found under view -> grid settings.

Note however that this changes the grid not the coordinate system. (I assume you had hopes that there is a way to set the coordinate system. I kind of assume you already knew about the grid origin)


I generally use the grid origin with custom grid sizes quite often. Mostly however in the footprint editor as described in Tutorial: How to make a footprint in KiCad 5.1.x (From scratch)? (The user grid and grid origin trick is used for the full molex connector tutorial.)

@Rene_Poschl are there “standard” or default grid sizes for:

  • Schematic sheets
  • Schematic symbols
  • footprint library
  • PCB layout (I recognize this may also depend on the fab house)

If you know: where is the definitive documentation for each of these grid sizes?

Great! This might perhaps be the easiest way to draw the edge cuts.
I 'd search for the discussion thread.
Thanks and best regards

:slight_smile:

I see your jokey face :slight_smile: That looks good for perhaps the defaults in source code, but what about for ease in connecting to standard symbols and footprints?

I could not find a tool on the right toolbar to change the grid origin.

Yes, the two-dimensional coordinate system. I assume that its origin is in either mm or in., whichever unit the user last chose. Isn’t “the grid” a set of parallel lines (that is to say, parallel to the x and y axes of this coordinate system ) set apart by a distance called the “grid spacing” ?
I see that this “grid spacing” can be selected from a menu of possible values. I further see that its current (x,y) value is displayed in the bottom right of the pcbnew viewport.

Do you recommend to start board layout using the default value of grid spacing ? I suppose this might vary with the needed density of traces/troughs in the area with the most-dense traces.

Talking about units for the coordinate origin makes no sense. The origin is simply the point (0, 0) of the coordinate system (0 is the same in all units).
In KiCad version 5 and earlier this center is always at the top left corner of the page. Any coordinate you enter into a properties dialog (like the properties of a line) is always relative to that origin.

The grid simply defines snapping points for KiCad tools. It can be displayed as lines, small plus signs or as dots. And yes the spacing is what defines how close together these snapping points are.

You can select spacings from a predetermined list or you can set a custom spacing in the grid settings dialog (the custom spacing can be different in x and y direction. It is only active if you select “user grid” from the standard list)

Another parameter of the grid is its starting point. This is especially noticeable for large grids like when using the custom grid for defining the board outline. The grid repeats with its spacing forever. But the place of the first point can influence which points you can snap to. For simplicity lets look only at the x axis. If you set the origin at 1mm and spacing at 5mm then you can reach points 1, 6, 11, … If you set origin to 0.5 then you can reach 0.5, 5.5, … But if you have the spacing as 0.5mm then these two origins do not change which points can be reached (both can reach 0, 0.5, 1, …)

1 Like

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