Profile toolpaths: inside, outside or on the line
A profile follows an outline with the tool offset to one side. Cut outside the line to keep the shape at its drawn size. Cut inside the line for a hole that a part must fit into. On the line splits the difference and loses half the bit diameter from each side.
Inside, outside, or on the line
The tool has width, so the software has to decide which side of your drawn line to put it on. Getting this wrong is the single most common cause of a part that is the wrong size.
| Setting | Tool runs | Result | Use for |
|---|---|---|---|
| Outside | Just outside the line | The shape stays exactly as drawn | Cutting a part out |
| Inside | Just inside the line | The hole is exactly as drawn | Cutting an opening something must fit through |
| On the line | Centred on the line | The shape loses half the bit diameter on each side | Scoring, single line grooves, V-groove folds |
With a 1/4 inch bit, a 2 inch square drawn and cut on the line comes out 1.75 inches. This surprises people every time.
Inside corners are round
A profile cut into an inside corner leaves a radius equal to half the cutting diameter. There is no way around it with a round tool. Three answers:
- Design the radius in, so the corner looks intentional.
- Use a dogbone or T-bone relief, a small extra circle cut into the corner so a square mating part still seats. Standard practice for CNC joinery.
- Use a smaller bit for the corners only, via a rest machining pass.
Tabs
A part that is fully cut out is free to move, and a free part under a spinning bit gets thrown. Tabs are small uncut bridges that hold it until the job is over. Place them on edges you will clean up anyway, avoid corners, and use more of them than you think for small parts.
Allowance and a finishing pass
Leave a small allowance on the profile during roughing, then run the same profile again at full depth with the allowance set to zero. The finishing pass takes almost nothing, so the tool barely deflects, and the wall comes out square instead of tapered. On a hobby machine this is the difference between a part that looks machined and one that looks routed.
Cutting through: where to put the bottom
Set the cut depth slightly deeper than your material, usually by 0.01 to 0.03 inches, so you go fully through even where the sheet is not perfectly flat. That means cutting into the spoilboard, which is what it is there for.
Common problems
| Symptom | Usual cause |
|---|---|
| Part is undersize by exactly the bit diameter | Cut on the line instead of outside |
| Part is undersize by two bit diameters | Offset went to the wrong side, inside instead of outside |
| Part is off by about half a bit diameter, or some odd amount | The bit diameter entered in CAM does not match the bit in the collet. Measure it. |
| Part is slightly undersize everywhere | Actual bit diameter is smaller than the value in CAM. Measure it. |
| Walls are tapered | Tool deflection. Add a finishing pass and reduce stickout. |
| Cut does not go all the way through in places | Stock is not flat, or Z zero is off. Increase the cut depth slightly. |
| Bottom edge splinters | Wrong bit for the material. See upcut versus downcut. |