Mill into frame for better board outline

[usbalbin]

Hi,

Sorry if this has been asked before. Note sure what to search for.

Let's say i have a board with an outline like this:

test_for_kikit/test_for_kikit.kicad_pcb

(kicad_pcb
	(version 20240108)
	(generator "pcbnew")
	(generator_version "8.0")
	(general
		(thickness 1.6)
		(legacy_teardrops no)
	)
	(paper "A4")
	(layers
		(0 "F.Cu" signal)
		(31 "B.Cu" signal)
		(36 "F.SilkS" user "F.Silkscreen")
		(44 "Edge.Cuts" user)
	)
	(setup
		(pad_to_mask_clearance 0)
		(allow_soldermask_bridges_in_footprints no)
		(pcbplotparams
			(layerselection 0x00010fc_ffffffff)
			(plot_on_all_layers_selection 0x0000000_00000000)
			(disableapertmacros no)
			(usegerberextensions no)
			(usegerberattributes yes)
			(usegerberadvancedattributes yes)
			(creategerberjobfile yes)
			(dashed_line_dash_ratio 12.000000)
			(dashed_line_gap_ratio 3.000000)
			(svgprecision 4)
			(plotframeref no)
			(viasonmask no)
			(mode 1)
			(useauxorigin no)
			(hpglpennumber 1)
			(hpglpenspeed 20)
			(hpglpendiameter 15.000000)
			(pdf_front_fp_property_popups yes)
			(pdf_back_fp_property_popups yes)
			(dxfpolygonmode yes)
			(dxfimperialunits yes)
			(dxfusepcbnewfont yes)
			(psnegative no)
			(psa4output no)
			(plotreference yes)
			(plotvalue yes)
			(plotfptext yes)
			(plotinvisibletext no)
			(sketchpadsonfab no)
			(subtractmaskfromsilk no)
			(outputformat 1)
			(mirror no)
			(drillshape 1)
			(scaleselection 1)
			(outputdirectory "")
		)
	)
	(net 0 "")
	(gr_arc
		(start 150 55)
		(mid 146.464466 53.535534)
		(end 145 50)
		(stroke
			(width 0.05)
			(type default)
		)
		(layer "Edge.Cuts")
		(uuid "5300d865-f3fe-45b9-bf04-ec36309b087e")
	)
	(gr_arc
		(start 105 50)
		(mid 103.535534 53.535534)
		(end 100 55)
		(stroke
			(width 0.05)
			(type default)
		)
		(layer "Edge.Cuts")
		(uuid "693cb5d6-984f-4237-99ce-ffaa15aafa1d")
	)
	(gr_arc
		(start 121 98)
		(mid 125 96)
		(end 129 98)
		(stroke
			(width 0.05)
			(type default)
		)
		(layer "Edge.Cuts")
		(uuid "78e9f83d-693f-470b-a2db-45f552f99a91")
	)
	(gr_line
		(start 145 100)
		(end 133 100)
		(stroke
			(width 0.05)
			(type default)
		)
		(layer "Edge.Cuts")
		(uuid "8a2069bf-97b5-45fe-9039-5d99b2fe5a29")
	)
	(gr_arc
		(start 133 100)
		(mid 130.763932 99.472136)
		(end 129 98)
		(stroke
			(width 0.05)
			(type default)
		)
		(layer "Edge.Cuts")
		(uuid "94176b5f-825a-43c5-876e-264409af37d8")
	)
	(gr_line
		(start 117 100)
		(end 105 100)
		(stroke
			(width 0.05)
			(type default)
		)
		(layer "Edge.Cuts")
		(uuid "a616a2b7-67ac-4aef-9814-b36652c59f40")
	)
	(gr_arc
		(start 145 100)
		(mid 146.464466 96.464466)
		(end 150 95)
		(stroke
			(width 0.05)
			(type default)
		)
		(layer "Edge.Cuts")
		(uuid "a629263e-720b-497d-99bf-0c81ca219fdb")
	)
	(gr_arc
		(start 100 95)
		(mid 103.535534 96.464466)
		(end 105 100)
		(stroke
			(width 0.05)
			(type default)
		)
		(layer "Edge.Cuts")
		(uuid "a6f9f7ba-cba5-47b7-8a7d-d278558b622f")
	)
	(gr_line
		(start 150 95)
		(end 150 55)
		(stroke
			(width 0.05)
			(type default)
		)
		(layer "Edge.Cuts")
		(uuid "af81f618-96b5-4517-a76e-8ea2519be16c")
	)
	(gr_line
		(start 100 55)
		(end 100 95)
		(stroke
			(width 0.05)
			(type default)
		)
		(layer "Edge.Cuts")
		(uuid "b6b0b069-641a-4cec-ad1b-116f99d2d998")
	)
	(gr_line
		(start 145 50)
		(end 105 50)
		(stroke
			(width 0.05)
			(type default)
		)
		(layer "Edge.Cuts")
		(uuid "e93c57e3-a4bb-401b-a908-1b67cefa02d2")
	)
	(gr_arc
		(start 121 98)
		(mid 119.236068 99.472136)
		(end 117 100)
		(stroke
			(width 0.05)
			(type default)
		)
		(layer "Edge.Cuts")
		(uuid "f0d907fa-22ba-4c1c-9f13-b4057193b853")
	)
	(gr_text "Test123"
		(at 117 77 0)
		(layer "F.SilkS")
		(uuid "3c4351bc-1736-4c83-9e8e-328f948e7029")
		(effects
			(font
				(size 3 3)
				(thickness 0.15)
			)
			(justify left bottom)
		)
	)
)

now I want to panelize this with 2x2 and v-cuts:

kikit panelize \
    --layout 'hbackbone: 5mm; vbackbone: 5mm; rows: 2; cols: 2' \
    --tabs 'type: full' \
    --cuts 'type: vcuts; layer: 0' \
    --framing 'type: tightframe; hspace: 0mm; vspace: 0mm; fillet: 2mm' \
    --fiducials 'type: 3fid; hoffset: 2.5mm; voffset: 10mm; opening: 2mm; paste: True' \
    --post 'millradius: 1mm' \
    'test_for_kikit/test_for_kikit.kicad_pcb' panel.kicad_pcb

Due to the mill radius of 1mm, I will get a board outline that fits quite poorly with what I intended. Is there any way to tell kikit to mill further into the framing to allow a better fit? As I see it, it would be possible to instead of stopping at the v-cut, continue milling furter inte the frame to better follow the intended outline. I would prefer to avoid mouse bites.

[yaqwsx]

There is a tab parameter cutout that adds extra space for the pockets. However, I am unsure at the moment how well it works with the tightframe option.

[usbalbin]

Thanks! I do not have access to the CLI right now and that does not seem to be available from the KiCad plugin. I will give that a try later when on another computer. In the mean time I managed to get it working with annotated tabs.

Here is a bit of my real board:

Will try to give the cutout thing a try as soon as possible.
Thanks a lot! :)

[yaqwsx]

The missing options were fixed in cc6f4dc.

[usbalbin]

Thanks a lot! Wow!

kikit panelize \
    --layout 'hspace: 2mm; vspace: 2mm; rows: 2; cols: 2' \
    --tabs 'type: full; patchcorners: False' \
    --cuts 'type: vcuts; layer: F.Cu' \
    --framing 'type: frame' \
    --post 'millradius: 1mm' \
    'test_for_kikit.kicad_pcb' 'test_for_kikit/panel2.kicad_pcb'

Edit: Just noticed that the cutout at the bottom could be a bit smoother. I might try some settings and see if i can get it even better

[usbalbin]

Slightly larger cutout and spacing between the boards and the outline is even better!

kikit panelize \
    --layout 'hspace: 5mm; vspace: 5mm; rows: 2; cols: 2' \
    --tabs 'type: full; cutout: 2mm; patchcorners: False' \
    --cuts 'type: vcuts; layer: F.Cu' \
    --framing 'type: frame; hspace: 2.5mm; vspace: 2.5mm; width: 2.5mm; fillet: 2mm' \
    --fiducials 'type: 3fid; hoffset: 2.5mm; voffset: 12mm; opening: 2mm' \
    --post 'millradius: 1mm' \
    'test_for_kikit/test_for_kikit.kicad_pcb' 'test_for_kikit/panel2.kicad_pcb'