Part Surface Differences in CNC Machining: 6 States and Their Fixes

• 1
  Six part surface differences, compared
• 2
  How to read a surface before you change a program
• 3
  Chatter and tool marks: vibration versus feed
• 4
  Burrs and burnish: two opposite failures
• 5
  Pitting and smeared metal: when the edge or the coolant fails
• 6
  Finishing choices: as-machined, ground, or coated
• 7
  What each fix costs in cycle time and setup

Surface condition is a measurement, not an opinion. Put the part under a 10× loupe and look at the spacing between marks. Even spacing means the marks come from the feed per tooth, so the fix sits in the speed and feed table. Uneven spacing, or marks that fade in and out along one wall, means the tool or the fixture is moving. That is a different problem and a different fix.

Measure the roughness before you touch anything. A hand-held profilometer reading across the lay gives you a number such as Ra 1.6–3.2 μm for a standard as-machined face. If the drawing calls for Ra 0.8–1.6 μm and you are reading 2.4 μm, you have a defined gap to close instead of a guess.

Look at where the bad zone sits. A band at mid-depth on a deep wall usually means the tool was deflecting as it entered. A band near the top only means the cutter rubbed on the first pass before it reached a stable chip load. Same part, two different corrections.

Finally, check the material before blaming the cutter. 6061-T6 cuts clean with a sharp edge and a healthy chip load. Soft 5052 and pure copper gum up unless the cutting edge stays sharp and the coolant reaches the tip. Part surface differences often track the alloy, not the machine.

Chatter is vibration, and it leaves a regular wave pattern that you can feel with a fingernail. The frequency tells you where it comes from. High-frequency chatter on a thin wall is usually the workpiece ringing. Lower-frequency chatter on a long reach is the tool bending. Both are stiffness problems, not speed problems, so raising the spindle speed rarely removes them.

The fix order matters. Shorten the tool overhang first, because rigidity falls with the cube of the length. Moving from a 4× to a 3× length-to-diameter ratio can cut deflection by more than half. If the part still rings, add a support or change the clamping so the wall is backed up during the finishing pass.

Tool marks are simpler. Evenly spaced lines come from the feed per tooth relative to the corner radius. A 6 mm cutter with a 0.8 mm corner radius at 0.05 mm per tooth leaves a scallop height you can see under a loupe. Halving the feed per tooth halves the scallop height and improves Ra, at the cost of cycle time.

Do not chase both at once. Settle the vibration first, then tune the feed. A program that is smooth but has visible marks still meets many drawings; a program with chatter often fails the tolerance as well as the finish.

Burrs form where the tool exits the material. The edge is unsupported on the last pass, so it bends instead of shearing. The size of the burr depends on the exit angle and how dull the edge is. A sharp tool with a clean exit can leave a burr small enough to remove in a vibratory tumbler. A dull tool leaves a burr that has to be deburred by hand.

You can reduce burrs in the program. Add a chamfer pass at the exit edge, or change the direction so the cutter exits into a sacrificial face. On cross holes, drill from the side that puts the breakout on a face you are going to machine anyway. These changes cost little and remove a manual operation.

Burnish is the opposite problem: the tool rubs instead of cutting. You see a bright, smeared band with no real chip. It happens when the feed per tooth drops below the minimum chip thickness, often around 0.01–0.02 mm for a sharp carbide edge. The edge cannot bite, so it polishes the surface and work-hardens it.

The fix for burnish is counterintuitive: feed harder. Raise the feed per tooth until a real chip forms, and the smeared band disappears. Then check the drawing tolerance, because a heavier chip load also raises cutting force. On thin features, solve the stiffness problem first.

Pitting shows as small dark spots on a machined face. Most of the time it is built-up edge. Material welds to the cutting edge, grows, then breaks off and takes a piece of the surface with it. Aluminium and stainless are the usual suspects. Raising the cutting speed slightly and increasing the coolant flow to the tip usually clears it.

Stainless 304 and 316 work-harden fast. If the tool dwells, the surface hardens under the edge and the next pass tears instead of cutting. Keep the cutter moving, take a real depth of cut, and never let the tool rub at the start of a pass. A minimum depth of 0.2 mm on finishing passes avoids the hardened skin.

Smeared metal on aluminium is a coolant and geometry problem. Two-flute cutters with a low helix clear chips poorly in a pocket, so chips recut and weld to the wall. A three-flute cutter with a higher helix and a flood or MQL supply leaves a clean wall and lets you run a higher feed per tooth without chatter.

When the same surface defect keeps returning across different jobs, suspect the material batch or the tool coating. Ask for the mill certificate and check the temper. A batch of 6061 that is not fully T6 machines gummy no matter what you do to the program.

An as-machined face at Ra 1.6–3.2 μm suits brackets, housings and most internal features. It costs nothing extra because it comes off the machine. If the drawing only calls out a general finish note, this is what you should expect, and it is enough for parts that bolt to something else.

When the drawing calls for Ra 0.8–1.6 μm, a finer finishing pass with a smaller stepover and a sharp, coated cutter usually gets there without a second operation. Below that, around Ra 0.2–0.8 μm, you are into lapping, honing or a finishing pass on a dedicated machine. Choose that route only where the function needs it, such as a seal face or a sliding bore.

Decorative and functional coatings change the picture. Anodizing builds roughly 0.005–0.025 mm per surface depending on the type, so anodize after you hold a tight dimensional tolerance, not before. Hardcoat anodizing adds more and can round a sharp edge. Bead blasting hides tool marks but also blurs a sharp corner.

For parts that must look uniform, a light bead blast or a tumble finish gives a consistent matte face across a batch. For medical and food-contact parts, passivation or electropolishing removes free iron and leaves a surface that cleans properly. Match the finish to the function and the inspection method, not to a photograph.

Every fix trades something. Shortening tool overhang may force a second setup for a deep pocket. Halving the feed per tooth to improve Ra can add 30–60% to the finishing cycle. A tumbler or bead blast adds a handling step and a day to the schedule, but removes manual deburring labor.

The cheapest fix is usually the one made before the cut. Choose the cutter and the holder for the feature, not for the tool crib. On a 4,000 mm part with long reach, a stub holder and a tapered tool can remove chatter that no speed change would touch. On a small 500 × 310 × 200 mm envelope part, a smaller cutter with a shorter flute length does the same job.

Plan the inspection too. If 100% inspection is required, roughness and burr checks add time per part. A profilometer trace on one feature per batch is enough when the process is stable, but a new setup deserves a full check on the first piece. Reports can be supplied on request.

Ask the shop what actually drives cost on your part. A finish callout that is one grade too fine can double a cycle, and a deburr note that can be met in the machine saves a manual station. Those two decisions usually matter more than any single cutting parameter.