How to Dogbones for CNC Machines
A dogbone is a small relief added to an internal corner so a round cutter can clear material a square edge needs. This guide shows how to size, place, and check them before you cut metal.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
Key takeaways
How to dogbones for CNC machines: the tool radius problem
Every end mill is a cylinder with a corner radius, even one sold as sharp. When the tool rolls into a pocket corner, the center of the cutter stops one radius short of the wall. The result is uncut material in the corner, shaped like the tool profile. That leftover is not machine error. It is geometry.
A pocket drawn with a true 90° internal corner cannot be milled by a round tool. The best a 6 mm end mill will do is a 3 mm corner radius. If a mating part has a sharp square edge, it will hit that radius and sit proud by 3 mm. A dogbone removes the interference.
The relief is a small circular extension placed on the corner bisector. Its diameter matches a cutter the shop will actually run. Once the dogbone is in the model, the toolpath clears the corner and the mating part seats flat.
This is the fastest fix in the file, and it is also the one most often missed. Designers who check corners at 5× in CAD catch it before a tool ever touches metal.
Sizing a dogbone relief from the tool radius
Size the dogbone from the cutter, not from the mating part. If the smallest end mill you want to run is 3 mm, the dogbone radius is 1.5 mm. If you can tolerate a 6 mm cutter, the radius is 3 mm. Smaller cutters reach deeper into corners but cost cycle time and break more often.
A practical floor for aluminum and brass is a 1 mm radius. Below that, tool life drops fast and chatter rises. In 17-4PH or Inconel, stay at 2 mm or larger unless the feature is shallow. Hard steel punishes thin tools at any depth.
Depth of the relief should match the depth of the feature. A dogbone 0.5 mm deep in a 12 mm pocket does nothing. Cut the relief through the full corner depth, or to the depth where the mating part sits.
Add a small clearance margin, 0.05–0.10 mm, beyond the nominal radius. That covers tool runout and keeps the corner from acting as a light press fit. Do not overdo it. A loose dogbone can let a pin rock in the pocket.
Deciding where how to dogbones for CNC machines applies
A dogbone belongs at any internal corner where a square or rectangular feature must seat fully. Slots for keys, pockets for square inserts, relay cutouts, and dowel-block recesses are common cases. Where the corner is only decorative or covered by a weld, skip it.
Two conditions must both be true. First, the corner is internal, formed by two walls meeting inside the part. Second, something with a square edge has to reach that corner. If a round pin or a loose-fit cover is the only thing going in, a normal corner radius is fine.
There is a third case worth naming. When a broached or EDM-cut square feature meets a milled pocket, the relief keeps the two operations consistent. Without it, the milled corner stands proud of the broached wall and the assembly binds.
On 5-axis parts, a dogbone on the corner bisector works the same way. The tool still has to reach the corner with its shank clear of the wall. Check the holder and the tool length in the simulation, not just the cutter diameter.
Stress, sealing, and when not to use a dogbone
A dogbone is a notch, and notches concentrate stress. In a static bracket that sees no load, the effect is negligible. In a part under cyclic load, a sharp-edged relief can start a crack at the corner. Use a full-radius relief so the tip is round, not pointed.
If the joint has to seal, a dogbone gives fluid a path around the corner. That matters on hydraulic blocks and vacuum manifolds. In those parts, keep the corner radius and adjust the mating part instead, or add an O-ring groove that swallows the radius.
Thin walls are the other limit. A dogbone removes material right where the wall is already weakest. If the wall is under 1.5 mm thick, check the section after the relief is added. Sometimes the answer is a thicker wall, not a smaller dogbone.
When the mating part can be changed, changing it is usually cheaper. Giving the mating part a matching corner radius costs a line change in its own model. Adding reliefs to a complex pocket costs machine time on every part.
How to dogbones for CNC machines in 6 steps
Work through the model in this order.
- 1Find the critical cornersList every internal corner that a square edge must reach. Mark them in the model with a colored sketch so you can count them later.
- 2Pick the cutterChoose the largest end mill that still reaches the feature depth. Its radius sets the dogbone radius: 3 mm cutter, 1.5 mm radius.
- 3Draw the reliefSketch a circle of that radius centered on the corner bisector, offset so the circle just passes the corner point. Trim the pocket boundary to it.
- 4Add clearanceGrow the circle by 0.05–0.10 mm for runout. Keep the growth the same on all corners so the part stays symmetric.
- 5Check the simulationRun the toolpath at 5× zoom. Look for a thin sliver of stock left at each corner, and confirm the holder clears the opposite wall.
- 6Note it on the drawingCall out the dogbone radius and depth in the notes, for example: dogbone R 1.5 mm, full depth. This stops a re-quote from removing them.
When a dogbone helps and when it does not
Match the case to the corner treatment.
| Case | Corner treatment | Reason |
|---|---|---|
| Square key in a milled slot | Dogbone relief | Key must reach the corner |
| Round pin in a pocket | Standard radius | Pin does not touch corners |
| Sealing hydraulic block | Keep radius | Relief would leak |
| Cyclic-loaded bracket | Full-radius relief | Reduces stress concentration |
| Decorative internal corner | Standard radius | No mating square edge |
| Broach meets milled wall | Dogbone relief | Keeps both walls flush |
| Wall under 1.5 mm thick | Review section first | Relief weakens the wall |
Fix the corners in CAD, not on the bench
Add dogbones only where a square edge must seat, size them from the cutter you are willing to run, and call them out on the drawing. Send the model early and we will check the corners in DFM before programming starts.
Dogbone questions engineers ask
How deep should a dogbone be cut?
Cut it to the depth of the feature it serves. If the mating part sits 8 mm into a pocket, the relief runs the full 8 mm.
A shallow dogbone only clears the top of the corner and leaves stock lower down. The part then seats at an angle, which is worse than not seating at all.
Can a dogbone be added after the part is machined?
Only if the corner has not been hardened or finished. A second milling pass with a small cutter can clear the corner, but the setup has to repeat exactly.
For anodized or plated parts, the extra cut breaks the coating at the corner and the finish has to be redone. Add the relief before the first cut.
Does every internal corner need one?
No. Most internal corners in a machined part are fine with the natural tool radius. Add a dogbone only where a square edge has to reach the corner.
If you dogbone every corner, you add cycle time and create stress risers you do not need.
What radius should I specify on the drawing?
Specify the radius you want the shop to run, not the tool size. A note of dogbone R 1.5 mm full depth tells the programmer the cutter limit.
If the corner is not critical, write a maximum radius instead, such as R 3 mm max. That gives the shop room to use a stiffer tool.
Will a dogbone raise the part price?
It can add a finishing pass with a smaller cutter, which costs cycle time. The increase is usually small next to the cost of a part that will not assemble.
Send the model early. A DFM review before programming catches missing corners while the fix is still free.
How do dogbones differ on a lathe?
Turning does not produce square internal corners, so the same relief does not apply. The nearest case is a milled flat or slot on a turned part.
Those features follow the same rule as milling: the cutter radius sets the corner radius, and a relief clears it.
Send your model for a corner check
Upload the CAD file and we return a quotation with free DFM analysis within 12 hours.
12-hour quote100% inspectionNDA on request
More machining notes
We publish setup notes, tooling trials and inspection data from the factory floor.
