Designing Inside Corners for CNC Machining: The Dog-Bone Trick

Why Inside Corners Can't Be Square

A CNC milling end mill is a rotating cylindrical tool. As it traces along the inside walls of a pocket, the tip of the tool follows the programmed toolpath — but where two walls meet at a 90-degree corner, the tool centre cannot physically reach the vertex. The result is an involuntary radius at every inside corner equal to the tool radius being used.

If your 8mm end mill is cutting a pocket, every inside corner will have an 4mm radius (half the tool diameter). This is physics, not programmer error. The only ways around it are to use a smaller tool (which takes longer and may not be practical for deep pockets) or to modify the design to accommodate the radius.

For most pockets, this is fine — a 0.5mm corner radius in an open pocket changes nothing functionally. The problem arises when the pocket must accept a mating part with sharp outside corners. A plate with 90-degree outside corners cannot sit flat in a pocket with inside corner radii — it will "float" on the corners, misaligned and rocking.

When It Actually Matters

Before learning the fix, it's worth being clear about when inside corner radii are actually a problem:

It DOES matter when:

• A mating part with sharp outside corners must fit into the pocket (e.g., a PCB slot in an enclosure, a square insert, a keyed slot)
• The pocket is part of a sliding fit where the insert must travel without interference
• The pocket receives a press-fit insert and the corners must be clear for correct seating
• The feature is a T-slot or dovetail with a precise profile that can't tolerate additional material at corners

It DOESN'T matter when:

• The pocket holds a round component, spring, or cylindrical insert
• The corners are purely cosmetic and nothing mates there
• The inside corner is a structural fillet — corner radii actually improve fatigue life
• The mating part will be machined to match (just tell the machinist to match corner radii)
• The pocket is large enough that the corner radius is negligible relative to the feature size

The Three Relief Options

When you need a square inside corner (or as close as possible), there are three approaches:

Option 1: Use a Smaller End Mill at the Corners

The machinist can do a "corner pass" with a smaller tool to reduce the corner radius. An 8mm roughing pass followed by a 2mm finishing pass at corners can reduce the radius from 4mm to 1mm. This works, but adds cost and machining time, and for very tight corners may require very small, fragile tools. Don't rely on this option without talking to your machinist — they may not offer it by default.

Option 2: Undercut the Corner (Square Undercutting Tool)

Specialty T-slot or undercutting end mills can create a near-square corner by undercutting slightly into the wall at the corner. This is expensive tooling and not available at every shop. It's used in aerospace and precision manufacturing but is overkill for most applications.

Option 3: Design in a Relief Feature (Dog-Bone, Tear-Drop, or Overcut)

This is the standard design-for-manufacturing approach: add a relief feature at each inside corner that gives the round tool somewhere to go. The tool cuts the relief feature, the corner is clear, and the mating part seats perfectly. Three variants exist:

• Dog-Bone Relief: A full circle drilled at the corner, centred on the corner vertex (or slightly past it). Visible outside the pocket profile but fully clears the corner.
• Tear-Drop (Lollipop) Relief: A circle positioned on the corner bisector, tangent to the pocket walls. More aesthetically compact than a dog-bone but slightly harder to program.
• T-Bone (Side Relief): The relief circle is positioned on the wall extension rather than on the diagonal. Good for slots and features with one preferred clearance direction.

Dog-Bone Geometry: The Math

The dog-bone relief is the most common and easiest to dimension. Here's the geometry:

For a simpler implementation, many designers just place the dog-bone centre exactly at the corner vertex. This works when the relief circle is slightly smaller than the tool diameter and when pocket position tolerance is liberal. But technically, centring the dog-bone on the vertex means the tool centre tracks the wall tangency point — the vertex of the pocket will be at exactly the corner point of the relief circle.

Visualising the Three Relief Types

Tear-Drop and T-Bone Variants

Tear-Drop (Lollipop) Relief

The tear-drop positions the relief circle on the bisector of the inside corner, tangent to both walls. The result is more compact — the relief circle doesn't protrude outside the pocket boundary as much as the dog-bone, and the appearance is cleaner. Tear-drops are preferred for appearance-sensitive parts and where adjacent features restrict the available clearance for a dog-bone.

The tear-drop's circle centre is at a distance of r / sin(θ/2) from the corner, where θ is the included angle of the corner. For a 90-degree corner: distance = r / sin(45°) = r × 1.414. For an 8mm tool: 4 × 1.414 = 5.66mm from the vertex along the bisector.

T-Bone Relief

The T-bone positions the relief circle centred on one of the wall lines, tangent to the perpendicular wall. This is useful when the inside corner is at the end of a slot and clearance is needed only in the length direction, not on the diagonal. T-bones are common in linear slot features where a sliding part enters from one direction.

Which to Use?

Choosing the Right Relief Radius

The relief radius should be based on the actual tool size your machinist will use for the pocket. The two critical rules are:

Rule 1: Relief Radius Must Be ≥ Tool Radius

If your relief circle is smaller than the tool, the tool still can't reach the corner. The minimum relief diameter equals the tool diameter. Most designers specify the relief radius slightly larger than the planned tool radius — a 10mm diameter hole for a 8mm end mill is a common choice.

Rule 2: Coordinate With Your Machinist

The "right" relief radius depends on what tools the shop actually has. A pocket 40mm deep will be cut with a longer reach end mill, which is available in limited diameters. Before specifying relief radii, confirm with your machinist what tool they plan to use for the pocket finishing pass. FYORD engineers review this when you submit a CNC order and flag any mismatches between your relief radii and our tooling inventory.

Implementing in SolidWorks and Fusion 360

In SolidWorks

There's no dedicated "dog-bone" tool in SolidWorks — you create them with standard sketch entities:

1. Sketch the pocket profile as normal
2. At each inside corner, draw a circle centred on the corner vertex (or on the bisector for tear-drops) with the appropriate diameter
3. Use Add Relation → Tangent or explicit dimension to position correctly
4. Merge the circle and the pocket profile using Trim Entities if you want a clean single-profile sketch
5. Extrude as a pocket

Alternatively, you can extrude the main pocket and then create a separate Extruded Cut for each dog-bone circle — this keeps the profiles clean and is easier to modify if you need to change the relief radius later.

In Fusion 360

Fusion 360 has a dedicated Dog-Bone feature in its Sheet Metal environment (for sheet metal parts). For machined parts, the approach is the same as SolidWorks — add circles to the sketch profile at corners. The Fusion 360 Script Library also has community-developed scripts that automatically add dog-bones to all inside corners of a selected sketch at a specified radius.

Automating Dog-Bones with Macros

For parts with many inside corners, manually drawing each dog-bone is tedious. Several free and paid SolidWorks add-ins automate this: DFMPro, DesignChecker, and community VBA macros. Search for "SolidWorks dogbone macro" — there are well-tested community scripts that detect all inside corners in a selected sketch and add the specified relief automatically.

Callout on Engineering Drawings

When sending parts to a machinist who will CAM your geometry directly, the dog-bones in your CAD model communicate the requirement automatically — they're part of the geometry. However, if you're sending a 2D drawing, include a general note:

If you require a near-square corner without a dog-bone (for aesthetic reasons or space constraints), note it explicitly: "INSIDE CORNERS: R0.5 MAX — SECONDARY PASS WITH 1mm END MILL REQUIRED." This way the machinist knows to plan for the extra operation and quote accordingly.

What About Laser-Cut Pockets?

Laser cutting is a 2D profiling process — it cuts through the full thickness of sheet metal in a straight vertical line. Unlike CNC milling, there's no rotation of the cutting tool, so laser-cut inside corners don't have the same tool radius problem. A laser beam focused to 0.1–0.3mm can cut very tight inside corners.

However, laser cutting is a 2D-only process. It cannot create pockets of varying depth, undercuts, or features that require 3D material removal. When you need pockets in plate or block material, you're in CNC territory. Laser is relevant for:

• Through-profiles in sheet metal (slots, holes, external profiles)
• Cut-outs in panels that mating parts pass through (not fit into at depth)
• Parts where the pocket is actually a through-hole and both sides are accessible

For a laser-cut slot where a mating part passes through the material thickness, you don't need dog-bones. The laser cuts the profile including inside corners to approximately the beam diameter (0.1–0.3mm radius). The mating part will seat without interference from corner radii — because laser inside corners are essentially sharp.

Quick Reference by Feature Type