CNC Machining Knife Overcutting: Causes and Controls
Corner gouges, scraped walls, and a tool that keeps cutting past the path are usually setup and control problems, not machine failure. This guide is for engineers and machinists who need to trace CNC machining knife overcutting to a root cause and correct it on the next run.
Overcut Symptoms, Causes, and Fixes
Match the mark you see on the part to the cause before you touch offsets.
| Symptom | Likely cause | First corrective action |
|---|---|---|
| Gouge at an inside corner | Tool radius larger than corner radius | Use a smaller cutter or leave a finishing allowance |
| Overcut only on one side of a slot | Runout or a bent cutter shank | Indicate the tool at 10 mm from the tip |
| Taper on a straight wall | Tool deflection under load | Reduce radial depth to 0.05 × D per pass |
| Overcut grows along the path | Losing steps on an open-loop axis | Check belt tension and motor current |
| Depth past the programmed floor | Z zero set on a rough surface | Re-zero Z on a clean, flat face |
| Oversize on the finishing pass | Worn or chipped cutting edge | Measure wear land, replace above 0.2 mm |
| Random gouges, no pattern | Workpiece movement in the fixture | Re-clamp and check clamp pressure |
Why the Tool Cuts Past the Path
Most overcutting is not the machine losing position. It is the cutter removing material the program never asked it to remove. On a 6 mm end mill running 2,400 rpm in 6061, a 0.02 mm radial deflection at the tip translates into a 0.02 mm oversize wall. That is already outside a ±0.005 mm callout, and nothing on the control display will show it.
Three things move material past the path: cutter deflection, cutter runout, and the corner geometry itself. Deflection scales with radial depth of cut and cutting force. Runout comes from the holder, the collet, or the shank. Corner geometry is fixed by the part drawing, so the only lever you have is the tool radius you choose to leave in it.
A fourth group is electronic. On a servo-driven machine, following error at high feed leaves a rounded entry and a gouged exit. On a stepper-driven router, a single missed step shifts every following move and the overcut grows as the path continues. The damage pattern tells you which group you are in.
Corner marks are geometric. Wall taper is mechanical. Growing overcut is electronic. Random marks are fixturing. Sort the symptom before you change a single offset.
Corner Radius and Tool Radius Mismatch
A cutter cannot enter a corner tighter than its own radius without leaving a witness. If the drawing calls a 1.5 mm inside radius and you finish with a 3 mm cutter, the toolpath either leaves a 1.5 mm fillet of uncut stock or the CAM system gouges the wall to fake the corner. Both outcomes look like overcutting to the inspector.
The rule on the floor is simple. Finishing cutter radius must be smaller than the smallest inside corner radius, and there should be a visible margin, not a tie. For a 1.5 mm corner, a 1.0 mm or 0.8 mm cutter gives the CAM system room to roll through without scraping.
When the corner is 0.5 mm or tighter, switch to electrical discharge machining or a 0.4 mm micro cutter with a light stepover. Pushing a 1 mm cutter into a 0.4 mm corner will chip the edge and gouge the wall in the same pass.
Check the drawing before the tool crib. Ten minutes with the corner radii list saves a scrapped part and a re-cut fixture.
Tool Runout, Offsets, and Z Zero
Runout is the quietest cause on this list. A 0.01 mm runout on a two-flute cutter makes one flute do most of the cutting. That flute pushes harder, deflects more, and cuts at a slightly larger effective radius than the other. The wall ends up oversize on one side of a slot and on size on the other.
Measure runout with a dial indicator at 10 mm from the tip, not at the holder face. Anything above 0.01 mm is worth fixing. Clean the collet taper, seat the cutter fully, and re-tighten to the holder's rated torque. A worn collet is a common cause and a cheap replacement.
Z zero is the other setup trap. Zeroing on a rough face, a burr, or a spot drill dimple sets the origin above or below the true surface. Every depth in the program then shifts by that error. Touch off on a clean, machined face, or use a tool setter and confirm with a 0.01 mm dial pass.
Wear offsets in the control drift over a run. If the operator updates the wear column without measuring the part, the finishing pass can remove 0.03 mm more than planned. Measure, then compensate, and log the value.
Servo Tuning, Step Loss, and Feed Rate
On a closed-loop machine, overcut that grows along a path points to following error and acceleration limits. A 90° corner taken at 3,000 mm/min asks the axis to reverse instantly. The servo lags, the corner rounds, and the control may overshoot on the exit. Dropping the corner feed to 800–1,200 mm/min with exact-stop or a fine tolerance mode removes most of it.
On an open-loop machine, step loss is the cause. A single missed step at 4,000 mm/min shifts all subsequent moves by that amount. You will see a clean wall on the first half of the part and an oversize wall on the second half, with a step change in between. Reduce rapid rates, check belt tension, and confirm the motor current is set to the driver's rating.
Feed rate interacts with deflection. Doubling feed roughly doubles cutting force and deflection, so a wall that was on size at 600 mm/min goes 0.03 mm oversize at 1,200 mm/min. For finishing passes in aluminium, 400–800 mm/min with 0.2–0.5 mm radial depth holds a ±0.005 mm wall on a rigid setup.
Warm-up matters on long runs. A spindle that grows 0.015 mm in the first hour moves the Z origin with it. Run a 15–20 minute warm-up cycle, then re-check the first part after an hour.
When the Material Pushes Back
Softer is not always easier. Aluminium 6061 machines clean, but it builds a built-up edge that acts like a second, larger cutting edge. The result is a wall that is oversize by 0.02–0.05 mm and a poor finish. Sharp, polished flutes and 8–12% coolant concentration keep the edge clean.
Stainless 304 and 316 work-harden. If the cutter rubs instead of cuts, the surface hardens and the next pass deflects off it into the wall. Keep the chip load above 0.02 mm per tooth, never dwell, and use a fresh edge for the finishing pass.
Titanium Ti-6Al-4V and Inconel push deflection much harder. Cutting force is roughly two to three times that of 6061 at the same chip load, so radial depth for finishing should drop to 0.05–0.1 × D. On thin walls, the part itself deflects away and springs back oversize. Support the wall from behind or take a spring pass.
Plastics behave differently. POM and PEEK expand with heat, so a wall cut at 3,000 rpm can measure oversize while warm and shrink on the bench. Use air blast, keep the feed up, and measure after the part reaches room temperature.
Step-by-Step Control of Knife Overcutting
Work in this order. Each step rules out one cause before you change offsets.
- 11. Map the overcutMeasure the oversize at three points: entry, middle, and exit of the cut. Write down the values. If the error grows along the path, go to step 5. If it is local to a corner, go to step 2.
- 22. Check corner radius against tool radiusList every inside corner radius on the drawing. Confirm the finishing cutter is at least 0.2 mm smaller. If not, change the tool, not the offset.
- 33. Indicate runout at 10 mm from the tipTarget below 0.01 mm. Clean the collet, reseat the cutter, re-torque. Replace any collet with visible scoring or a worn bore.
- 44. Re-zero Z on a clean faceTouch off on a machined flat, not on a rough surface or a drill dimple. Confirm with a 0.01 mm dial pass across the face before running the program.
- 55. Reduce corner feed and radial depthSet corner feed to 800–1,200 mm/min with exact-stop. For finishing, use 0.2–0.5 mm radial depth in aluminium and 0.05–0.1 × D in titanium or Inconel.
- 66. Take a spring passRun one finishing pass at the same offset with a 0.02–0.05 mm radial cut. This removes the deflection left in the wall without changing the programmed geometry.
- 77. Verify and logMeasure the part, record the wear offset you applied, and note the feed and depth used. Use the same numbers on the next run and check the first article again.
Overcutting Questions from the Shop Floor
Is overcutting caused by the machine or the program?
Usually the program and the setup, not the machine. Corner geometry, tool radius, runout, and Z zero account for most cases we see.
Machine-side causes appear as a growing error along the path or as a step change mid-part. Measure three points before you blame the control.
How small a corner radius can CNC machining hold?
On a 3-axis mill, a 0.5 mm inside corner is practical with a 0.4 mm cutter and light stepover. Below that, the cutter is fragile and deflection dominates.
For corners tighter than 0.4 mm, electrical discharge machining is the more stable route. We quote both when a drawing has tight corners.
Does coolant affect the wall size?
Yes, indirectly. Poor coolant flow lets a built-up edge form on aluminium, and that edge acts like a larger cutter. It can add 0.02–0.05 mm to a wall.
Keep concentration at 8–12% and direct the stream at the cutting zone, not at the chip pile.
What tolerance should I expect on a thin wall?
A wall under 1 mm thick deflects under cutting force even at light depths. Expect ±0.02 mm unless you support it.
Support from behind, take a spring pass, and finish with small radial depth. With those steps, ±0.005 mm is achievable on walls above about 1.5 mm.
How do I tell step loss from deflection?
Deflection gives a gradual taper and a smooth wall. Step loss gives a sudden shift, often paired with a visible witness line.
Run the same program at half the rapid rate. If the overcut disappears, it was step loss.
Can a finishing pass fix an already oversize wall?
No. Once the wall is oversize, the material is gone. You can only rework the part if the drawing allows a larger size or a weld-and-remachine route.
Prevention is cheaper. Check runout, corner radius, and Z zero before the finishing pass starts.
Send Us the Part That Keeps Overcutting
Upload the drawing and the problem area. We return a quotation and a free DFM analysis within 12 hours, with the tooling and feeds we would use.
12-hour quoteFree DFM analysis100% inspectionNo minimum order quantity
More from GreatLight
We publish setup notes, tooling trials and inspection data from the factory floor.
