I installed V5 a couple of days ago after purging 4.0.7 to avoid conflicts. The first application I tried was the special pad shape, shown in the attachment, which required hacks (overlapping trapezoids) in 4.0.7 and subsequent cleanup of the solder mask by hand. I defined the pad in question as “Custom (Rect. Anchor)” and entered the appropriate segments in “Custom Shape Primitives.” KiCAD insists on an anchor (what is that, exactly) and, although the segments are correct and form a closed polygon, only the anchor is shown as copper.
I did try to find some documentation on custom pad shapes before posting this, but I could not find any. The pad is essentially rectangular, but with a corner truncated along a straight line, but the resulting closed polygon is not a trapezoid. The dimensions, several of which are redundant but were included for convenience, are in mm. Is there any way to import the shape of the pad as, say, a DXF file?
The anchor is just a conventional pad (round or rectangular, TH or SMD). Electrical connections are made to it. The custom pad shape basically goes a round it, of course it needs to be connected by overlapping. Both the anchor pad and the custom shape should show up in the pad editor.
FreeCAD and StepUp plugin can be used to create and export DXF to KiCad. There’s enough information about it already in the internet and in this forum, but I bet someone here will give you more soon.
In KiCad you don’t have to edit polygon corners as numbers. Create a graphic polygon to some layer. Open its Properties and change the layer to the wanted copper layer. Create a normal rectangle or round pad and move it inside the polygon. Select both and open the context menu -> Create Pad from Selected Shapes.
Basically the additional normal pad exists just to give the pad a center point, i.e. an anchor (I think).
Draw a polygon over the pad on the FSilk.S layer. Here I used a grid size of 0.01mm, using the keyboard arrow keys and the relative position. I made the corner chamfer 0.33 x 0.31. Set the polygon line width to 0.0 mm.
Yes, you don’t have to move the polygon to a copper layer first, contrary to how I did it. I think earlier in nightly builds you had to do that, but at least in 5.0.0 it’s more simple.
importing a dxf in kicad fp atm is giving you a non filled pad.
A workaround can be done importing the dxf in FC and then use it with StepUp to convert the dxf to a polyline sketch wich will allow you to export a corresponding kicad fp.
@maui, @madworm, @eelik, @bobc: Thank you all. I think I now know my problem: In the “Custom Shape Primitives,” instead of adding individual segments, I should have added a polygon (this is the last selection from the top, requiring scrolling of the pop up menu to get to it) and then manipulated the corners of the polygon.
still import from DXF will not be converted to a polygon, but to single segments;
there is a button to import primitives (i.e. polyline from points) but this is still not implemented.
The option to import from dxf to create custom filled pad shapes (i.e. for RF design) is not viable atm inside kicad.
The only use I found is for this special footprint where there is an annular pad which can be done as a custom primitive “circle” with an assigned width
@bobc: Thank you for pointing out this very simple detail. Will the Python window be re-enabled in KiCAD5? I do remember reading in the forums that there was an issue with wxPython and its dependencies on GTK2.
@maui: Thank you for the interesting example. How did you come up with the stencil pattern on the right?
All primitives are able to create pads. However, only the polygon will be a filled pad. There are different use-cases for arcs/segments/circles that are not filled. However, they must all share an intersection with the anchor pad. i.e. all items in the custom footprint must be electrically connected.
