CNC Milling Tips: A Step-by-Step Guide to Accurate Parts

• 1
  Key takeaways
• 2
  Workholding and Setup: Where Most Accuracy Is Lost
• 3
  Tool Selection: Fewer Tools, Shorter Reach
• 4
  Feeds and Speeds: Start From Surface Speed
• 5
  In-Process Checks: Catch Drift Before the Finish Pass
• 6
  A Repeatable 7-Step Milling Procedure
• 7
  Starting Cutting Data by Material

Most out-of-tolerance parts are not cut wrong, they are held wrong. Before touching feeds, look at how the blank sits. A vise with 2 mm of jaw contact on a 100 mm tall part will move under load, and no amount of tool compensation fixes that.

For plate work, support the part across its full length. Parallels under the blank keep it off the vise floor and stop the cutter from pushing the part down. For thin walls under 2 mm, add a sacrificial backing plate or leave tabs, then cut them in a second operation.

Clamp pressure matters too. Aluminum 6061 will spring back if you crank a vise handle hard, and the finished width drifts 0.05-0.1 mm. Use a torque wrench on repeat setups, or switch to soft jaws machined to the part profile.

Zero the tool on the actual stock, not on the drawing. If the blank is 0.2 mm oversize, every depth cut is 0.2 mm deeper than programmed. Touch off on the stock face and adjust your Z offset once, before the first pass.

• 1
  Support the partFull contact under the blank, no overhang beyond the jaws.
• 2
  Control clamp forceSoft jaws or a torque wrench for repeatable clamping.
• 3
  Zero on real stockTouch off the blank, not the nominal surface.
• 4
  Plan the second opLeave tabs or a backing plate for thin walls.

A three-flute carbide end mill covers most aluminum work. It has enough flute volume to clear chips at high feed and enough rigidity to take a 0.5 × diameter axial cut. Two-flute tools are for slotting and plastics where chip clearance is tight.

Reach is the number that kills tools. A 6 mm cutter hanging 40 mm out of the holder will deflect under side load. If the geometry allows, step the part down and use a shorter tool with a smaller diameter instead of one long tool at full depth.

For steel and stainless, use four or more flutes with a TiAlN or AlTiN coating. The extra flutes raise feed per revolution at the same chip load. For Inconel and other nickel alloys, choose a geometry with a reinforced edge and run it slow.

Keep tool runout under 0.01 mm. A cutter with 0.03 mm of runout will cut one flute harder than the rest, and that flute fails first. Check with a dial indicator on a gauge pin in the collet.

Plastics need sharp, polished flutes. A standard aluminum cutter will melt POM and leave a burr on PMMA. Use an O-flute or a single-flute router bit at high rpm and fast feed.

• 1
  3 flutes for aluminumGood chip room, rigid enough for 0.5 × D axial cuts.
• 2
  Shorter is stifferKeep tool overhang below 4 × diameter when possible.
• 3
  Runout under 0.01 mmCheck the whole holder and collet assembly.
• 4
  O-flute for plasticsPrevents melting and stringy chips.

Work from surface speed, not from rpm. For aluminum 6061, 300-500 m/min is a safe band with carbide. For 304 stainless, 80-120 m/min. For Ti-6Al-4V, 30-50 m/min. Convert to rpm with rpm = (surface speed × 1000) ÷ (π × tool diameter).

Chip load sets the feed. A 6 mm three-flute cutter in aluminum wants roughly 0.05 mm per tooth, so feed = rpm × flutes × chip load. If the machine can hold that feed, the cut sounds steady. If it screams, reduce chip load before reducing rpm.

Depth of cut is the last dial to turn. Radial engagement around 40-50% of tool diameter and axial depth up to 1 × diameter works for aluminum in a rigid setup. Reduce axial depth to 0.3 × diameter on long-reach tools and on stainless.

Coolant choice follows the material. Aluminum runs dry or with mist if chip evacuation is good. Stainless, titanium, and Inconel need constant flood coolant to protect the edge. Cast iron is usually cut dry.

• 1
  Aluminum 6061300-500 m/min, dry or mist, 3-flute carbide.
• 2
  Stainless 30480-120 m/min, flood coolant, 4-5 flutes.
• 3
  Ti-6Al-4V30-50 m/min, high-pressure coolant, light axial depth.
• 4
  Inconel20-35 m/min, rigid setup, expect short tool life.

Measure after roughing while there is still stock left. If a wall is 0.15 mm off after the roughing pass, you can split the difference in the finishing cut instead of scrapping the part.

Thermal drift is real on long runs. A spindle that has been running for three hours will be warmer than a cold one, and the Z zero moves with it. Re-touch off on a known surface every few hours, or run a warm-up cycle at the start of the shift.

Chip recutting is the most common cause of poor finish on deep pockets. If the chip cannot leave the cut, the tool cuts it again, and the edge chips. Use air blast or through-tool coolant and program a retract every 3-4 passes on slots deeper than 4 × tool diameter.

For slots deeper than four times the tool diameter, reduce feed rate by about 20% to keep chip clearance stable. The same rule applies to deep ribs where the tool has to enter and exit repeatedly.

Hold tight tolerances with a finishing pass at full depth. Take 0.3-0.5 mm radial stock into one continuous cut rather than three spring passes, which rub the edge and polish the surface instead of cutting it.

• 1
  Measure mid-runCheck walls after roughing, not only at final inspection.
• 2
  Manage heatWarm up the spindle or re-zero after long runs.
• 3
  Clear chipsAir blast or through-coolant on pockets deeper than 4 × D.
• 4
  One finish passFull depth, 0.3-0.5 mm radial stock.