How to Manage Problems in CNC Treatment on the Floor

• 1
  Common problems in CNC treatment at a glance
• 2
  Overcut at corners and walls thinner than nominal
• 3
  Chatter marks, poor finish and rubbing in corners
• 4
  Uneven cutting margin on curved surfaces
• 5
  Tool wear, drift and what to check between parts
• 6
  A six-step routine to manage problems in CNC treatment

Overcut shows up as a wall that measures 0.03 mm under nominal, or a corner radius that reads larger than the drawing. The cut looks fine in the middle of a long straight section. It goes wrong where the tool changes direction. On a curved surface the side stock can be 0.5 mm while the floor stock is 0.15 mm. That difference is enough to push the tool sideways.

The first cause is uneven stock. A casting or forging that was supposed to leave 0.4 mm all round may leave 0.6 mm on one flank and 0.2 mm on the other. A finishing pass with a fixed radial depth then bites harder on the thick side. The tool deflects, and the wall gets thin. Measure the blank in three places before you write the finish pass.

The second cause is toolpath geometry. CAM software often keeps a constant feed through a corner, but the tool engagement angle rises sharply there. Radial engagement can jump from 10 percent to 40 percent of the cutter diameter in a 90 degree turn. The cutting force rises with it. A few spring passes, or a feed reduction at corners, removes most of the error.

A third factor is cutter selection. A long, thin end mill will deflect more than a stubby one. The rule we use is simple: as large as the geometry allows, as short as the holder allows. Where a deep pocket forces a long tool, plan a roughing pass with a larger cutter and leave the long tool for the light finishing cut only.

• 1
  Check stock firstWrite down the actual stock on two opposite sides before choosing depth of cut.
• 2
  Add spring passesTwo passes at the same offset take out deflection without changing the program.
• 3
  Slow the cornersReduce feed at arcs and sharp turns where engagement climbs.
• 4
  Keep the tool shortEvery extra 10 mm of overhang adds deflection at the same cutting load.

Chatter is a vibration, not a wear problem. It leaves evenly spaced marks on the wall. The spacing usually matches the tooth passing frequency. Once you hear it, the surface is already out of spec, so the fix has to happen at the setup or the program, not at the polishing bench.

The most common trigger is tool overhang. A 12 mm carbide end mill held 80 mm out of the holder will sing in most materials. Shorten the overhang to 40 mm and the same cut often goes quiet. When the geometry will not allow that, step down to a smaller diameter tool with a higher spindle speed, or use a tool with a different flute count to shift the natural frequency away from the tooth passing frequency.

Corner rubbing is a separate fault. It happens when the feed is too high for the arc radius, so the tool rubs instead of cutting. The marks look bright and smeared rather than torn. Reducing feed at the arc, and letting the control slow the corner through its acceleration settings, clears it. On older machines with no look-ahead, this has to be written into the program by hand.

Rigidity of the part matters as much as the tool. A thin floor or a tall rib will move under cutting force even with a perfect setup. Support the part with a soft jaw, a fixture block or a tailstock. Where the part is too flexible, take lighter depths and accept more passes.

• 1
  Shorten overhangHalving overhang raises stiffness by roughly eight times.
• 2
  Change the tooth frequencyA different flute count moves the vibration away from the cut.
• 3
  Feed down at arcsKeep chip load steady where the engagement angle rises.
• 4
  Support the partSoft jaws and fixture blocks stop the workpiece from moving.

Uneven margin is the quiet cause behind many of the other faults. On a curved surface, the side stock may be 0.5 mm while the floor stock is 0.15 mm. The finishing tool then has a different load on each pass. The result is a wall that is thin in one area and on size in another, and no single offset will fix both.

The cure starts in the roughing program. Use a constant engagement toolpath so the radial load stays within a narrow band. Where the CAM package does not support that, break the roughing into zones and check the remaining stock with a probing cycle or a caliper at three points. A ten minute check here saves an hour of rework later.

When the blank itself is uneven, as with castings and forgings, the first operation should establish a reference. Face one side, then use that face to locate the second operation. Trying to finish both sides from the raw surface leads to a part that is on size in the middle and thin at the edges.

For thin floors, leave 0.2 mm to 0.3 mm for the finishing pass and take it in two light cuts. Cutting the floor in one heavy pass pushes the material away from the tool and leaves a dished surface. Two passes at the same offset let the material spring back between them.

• 1
  Constant engagementKeep radial load steady through the whole roughing path.
• 2
  Establish a datumFace one side first, then locate the second operation from it.
• 3
  Light floor cutsTwo passes at 0.1–0.15 mm beat one heavy pass.
• 4
  Verify before finishingProbe or measure the stock so the finish pass is predictable.

Tool wear does not show up as a sudden failure. It shows up as a dimension that creeps. A slot that measured 12.02 mm at the start of the run reads 12.06 mm after 60 parts. The surface finish may still look acceptable, so the drift is easy to miss until a gauge catches it.

Set a measurement interval based on the tolerance band, not on the shift. For a part held to ±0.05 mm, measuring every 20 parts is usually enough. For a part held to ±0.005 mm, measure more often and record the readings so you can see the trend before the part goes out of tolerance. Adjust the wear offset in small steps and log each change.

Thermal growth is the other source of drift. A spindle that has been running for two hours is longer than a cold one. On tight work, run a warm-up cycle at the start of the shift and check the first part against the last. If the shop is not temperature controlled, the part itself will grow and shrink through the day.

In-process checks catch more than final inspection can. At our plants we check raw material before cutting, monitor critical dimensions in process and inspect 100 percent before shipment, with reports available on request. That sequence is what holds a ±0.005 mm tolerance over a production run.

• 1
  Measure on a scheduleBase the interval on the tolerance band, not the shift length.
• 2
  Warm up the spindleRun a warm-up cycle so the first part matches the last.
• 3
  Log the offsetsWrite down each wear adjustment and the part number it followed.
• 4
  Check material firstHardness and stock variation change the wear rate.