Dogbone and T-Bone Fillets for CNC Router Plywood Joinery: Corner Relief Math and Toolpath Setup

A round router bit cannot cut a square inside corner. When you rout a pocket or slot for a tab, the corner of the mating part hits the rounded corner left by the bit, and the joint will not seat. CNC joinery solves this with corner relief cuts, usually called dogbones and T-bones, that deliberately overcut the corner so square parts fit. This guide covers the geometry, how much to cut, and how to set it up in CAM.

Why Corners Need Relief

Assume a bit radius of r. When the bit follows the inside wall of a pocket, its centre stays r away from each wall. At a 90 degree corner the centre therefore sits at a distance of r times the square root of two from the corner vertex, which leaves an uncut fillet of the bit's radius. The tab's square corner is now interfering with that fillet. To fix that, the bit centre must be allowed to reach a point no more than r from the vertex, so the bit's circle covers the corner.

Dogbone vs T-Bone

TypeBit pathOvercut locationBest for Dogbone (diagonal)Bit centre plunges into the corner along the 45 degree bisectorVisible on both faces of the cornerHidden joints, small bits, parts where both walls stay covered T-bone (edge)Bit extends along one wall past the cornerOnly on one side, along a single wallJoints where one edge is visible and the other hidden

The Numbers

For a dogbone, move the bit centre along the diagonal until it sits on a circle of radius r around the vertex. In practice that means the centre ends about 0.707 times r past each wall, into the material. For a T-bone, extend the toolpath along one wall so the bit centre finishes directly above the adjacent wall's line (roughly one bit radius of extra travel). Add a small clearance of 0.05 to 0.1 mm to either so the corner does not touch the circle exactly.

Bit diameterRadius rDogbone centre offset past each wall (0.707 r)T-bone extra travel (r) 3.175 mm (1/8 in)1.59 mm1.12 mm1.59 mm 6 mm3.00 mm2.12 mm3.00 mm 6.35 mm (1/4 in)3.18 mm2.25 mm3.18 mm 9.525 mm (3/8 in)4.76 mm3.37 mm4.76 mm

Use a smaller bit to minimise the visible overcut. A 1/8 in bit leaves a much less obtrusive notch than a 1/4 in bit, at the cost of slower cutting and a higher risk of breakage.

Setup in CAM

1. Fusion 360: in 2D Pocket, expand the Passes tab and enable corner options where available, or add dogbone circles to the sketch geometry and pocket with those. Many users prefer drawing the relief circles directly into the sketch because it is predictable across machines.
2. Vectric (VCarve, Aspire, Cut2D): use the Dogbone or T-bone fillet add-in gadgets, which add relief to selected vectors based on the bit size you specify.
3. Free tools: Inkscape and FreeCAD have extensions and macros that generate dogbones on selected corners.

Alternative: Design Around the Corner

Instead of overcutting, some designers cut the mating tab with matching rounded corners, or chamfer the tab corners on the CNC after the fact. Rounded corners on the part are also cheaper because they need no extra toolpath. For structural joints, dogbone joints are stronger because the full flat faces of the tab still contact the wall.

Plywood Fit Tips

• Measure your actual plywood. Nominal 18 mm or 3/4 in plywood is rarely that thick, and thicknesses vary between sheets. Cut a test joint from an offcut and adjust the slot width in CAM.
• Use compression or downcut spirals as appropriate for the material to avoid chipout at the mouth of the slot.
• Allow 0.1 to 0.2 mm of extra slot width for a press fit, or 0.3 mm or more if you intend to glue.
• Cut slots first with a slower feed to avoid tab breakage. Add tabs to hold the parts in place.

Closing

Dogbones and T-bones add a few lines of geometry that turn a machine's rounded corners into an accurate joint. Pick the type by where you can hide the overcut, keep bits small when appearance matters, and always test on scrap before cutting a full sheet.