How to Operate a CNC Shaving Machine

• 1
  Key takeaways
• 2
  What a CNC shaving cycle actually cuts
• 3
  Setup checks before you press cycle start
• 4
  Speed, feed and in-feed ranges that work
• 5
  Faults you will see on the flank and what causes them
• 6
  How to operate a CNC shaving machine: step by step
• 7
  Shaving versus other gear finishing routes

A CNC gear shaving machine is a finishing machine. The workpiece is clamped between centers or in a fixture and rotates under power. The shaving cutter, a hardened disc with gashed teeth, is driven by the pin and turns in mesh with the gear at crossed axes. The crossing angle is usually 10–15 degrees, and that angle is what produces sliding velocity along the flank instead of pure rolling.

That sliding motion is the whole point. Hobbing leaves small feed marks and a periodic tooth-to-tooth error. Shaving shears off 0.002–0.02 mm of material per pass from the flanks and the root fillet, which corrects lead, profile and runout at the same time. It does not correct index error from a bad hob, and it does not fix a bent shaft.

Because the cut is light, the fixture matters as much as the cutter. If the part deflects 0.02 mm under cutting load, the flank comes out tapered. Check that the centers are clean, the tailstock pressure is steady, and the drive dogs sit tight. On thin-web gears, a face driver with a support ring beats a plain mandrel every time.

Typical cycle time on a 40-tooth spur gear is 20–60 seconds, including in and out feed. Shaving runs wet, with cutting oil or a low-viscosity neat oil. Sulfurized oil helps on 20MnCr5 and 8620, but it stains some non-ferrous parts, so confirm the fluid against the material before you commit a batch.

• 1
  Good candidateHobbed spur and helical gears, module 1–6, with 0.02–0.05 mm stock on the flank.
• 2
  Poor candidateHardened gears above roughly 350 HB, internal gears, and gears with no hobbed pre-cut.
• 3
  Shape mattersVery narrow face width under 5 mm gives the cutter almost no axial travel room.
• 4
  MaterialFree-cutting alloy steel shaves cleanly; soft aluminium gums the cutter and needs a different route.

Start with the cutter. Inspect the gashes for built-up edge and the tips for chipping under a loupe. A chipped tooth will print a raised line on the gear flank and you will find it only at final inspection. Measure the cutter outside diameter and record it. That number goes into the center distance calculation, and a 0.1 mm error there becomes a 0.1 mm error in tooth thickness.

Set the crossed-axes angle to the value in the process sheet, usually 10–15 degrees. On most machines this is a swivel of the cutter head, and the scale is not always accurate. Indicate the cutter face against a known surface if the machine has an adjustment. Then set the center distance so the cutter and the gear mesh with the backlash the process sheet calls for.

Clean both centers and the locating face. A chip under the part is a 0.01–0.03 mm runout error that no amount of parameter tuning will remove. Check tailstock pressure against the sheet; too little and the part walks, too much and the centers brinell the shaft ends on soft material.

Load the program and dry-run the cycle with the cutter retracted. Watch the in-feed, the axial traverse and the out-feed. On a CNC shaving machine the axial stroke per revolution is typically 0.1–0.3 mm, and the total stroke is set to clear the face width by 5–10 mm at each end. Confirm the numbers on the screen match the process sheet before any metal is cut.

Cutter speed on steel gears usually sits between 100 and 200 m/min surface speed. Harder or higher-alloy steel runs at the low end. If you see blue discoloration on the chips, you are running too fast for the coolant flow, not for the material. Shaving generates very little heat, so burn marks almost always trace back to a dry zone or a starved nozzle.

Radial in-feed per pass is 0.01–0.03 mm. Most shops split the total stock into two or three passes, with the last pass at half the in-feed of the first. That final light pass is what produces the fine finish, typically Ra 0.8–1.6 μm on the flank. One heavy pass of 0.05 mm will tear the surface and load the cutter.

Axial feed per revolution of the workpiece runs 0.1–0.3 mm. Higher feed shortens the cycle but leaves a coarser axial pattern. If the print calls for lead accuracy better than 0.008 mm over the face width, stay at 0.1–0.15 mm and accept the longer cycle. For general power transmission gears, 0.25 mm is a reasonable compromise.

Coolant flow should hit the mesh point, not the top of the part. Aim the nozzle so the oil enters the contact zone and flushes chips away. Recheck flow after every tool change. A partially blocked nozzle is the most common cause of a sudden finish drop in the middle of a production run.

Diagonal marks across the tooth flank mean the crossed-axes angle is wrong or the cutter is not square to the work axis. Recheck the swivel setting and indicate the cutter face. This fault often appears after a setup change and looks alarming, but it corrects quickly once the angle is right.

A shiny, burnished band near the root or tip is a sign of too much in-feed on a single pass. The flank is being rubbed rather than cut. Split the stock into three passes and drop the first in-feed to 0.015 mm. Check that the coolant reaches the mesh point before you change any other parameter.

Tapered flanks across the face width usually trace back to part deflection or a chip under the locating face. Inspect the fixture, the centers and the tailstock pressure. On long, slender gear shafts, add a steady rest or reduce the axial feed to 0.1 mm per revolution.

Tooth thickness drifting over a batch is cutter wear. Recheck the outside diameter every 50–100 pieces and adjust center distance to compensate. On a well-maintained machine, shaving can hold ±0.005 mm on tooth thickness across a run, but only if wear compensation is tracked.