DXF import line thickness

[moorejl57]

New to Kicad (Eagle deserter), running 4.05

I made a complex board outline in Onshape and then exported the sketch to dxf. When I try to import the dxf into the PCB editor, it seems to work with the exception of making all the line widths 2.54 mm (very thick). It is a real time burner to select each line segment and edit the width, am I missing an obvious way to control imported line thickness?

I have no problem importing Onshape dxf into footprint editor, all lines are expected thickness.

[maui]

Does anyone know how to set all the selected line widths in one go?

Is python accepted: import pcbnew board = pcbnew.GetBoard() for drw in board.GetDrawings(): if drw.IsSelected(): drw.SetWidth(int(0.1 * 1e6)) Above snippet sets line width for all selected drawing elements (lines etc.) to 0.1 mm. Note that 1e6 multiplier is required because internal units of kicad is nanometers.

Does anyone know how to set all the selected line widths in one go?

and this script is useful to change Layer of selected lines import pcbnew board = pcbnew.GetBoard() Dwgs_User=40 for drw in board.GetDrawings(): if drw.IsSelected(): drw.SetLayer(Dwgs_User) where Layers nbrs are: (0 F.Cu signal) (31 B.Cu signal) (32 B.Adhes user) (33 F.Adhes user) (34 B.Paste user) (35 F.Paste user) (36 B.SilkS user) (37 F.SilkS user) (38 B.Mask user) (39 F.Mask user) (40 Dwgs.User user) (41 Cmts.User user) (42 Eco1.User user hide) (43 Eco2.User user) …

[moorejl57]

That worked when run as a file with execfile in OpenGL view