CNC machining small parts: where the physics changes

• 1
  Why CNC machining small parts behave differently at the spindle
• 2
  Workholding is the first limit on small part accuracy
• 3
  Tool runout and micro-tool life on tiny features
• 4
  Material choice changes the small part window
• 5
  Burrs, edges and finishing on small parts
• 6
  How we verify small part dimensions
• 7
  Feature size versus what the process can hold

CNC machining small parts is not simply the same operation scaled down. Cutting speed, feed per tooth and radial engagement all come from tool diameter, and below Ø3 mm those numbers collapse fast. A Ø1 mm end mill needs high spindle speed to reach a sane surface speed, but the tool shank is thin enough to bend under loads that would be trivial on a Ø12 mm cutter.

The part is also weak. A 0.8 mm wide rib on an aluminum housing has almost no section modulus, so the force that removes material also deflects the feature being cut. Cutting pressure pushes the wall away from the cutter, the tooth takes a lighter chip, and the wall springs back once the tooth passes. The result is a dimension that measures wrong even though the machine itself is accurate.

Heat is the third variable. On a big part, chips carry most of the heat away. On a Ø2 mm cutter the chip is tiny, the tool has almost no thermal mass, and the same spindle speed that works on a larger tool will cook the edge. Small tools live or die by chip evacuation, not by rigidity alone.

None of this makes small part machining impossible. It means the process window narrows, and the shop has to trade material removal rate for control. That trade is the whole subject of this page.

• 1
  Tool diameter sets everythingSpeed, feed and depth of cut scale with it, not with part size.
• 2
  Deflection, not machine errorThin walls and thin tools bend under normal cutting loads.
• 3
  Heat concentratesSmall chips remove far less energy per revolution.

A 15 mm part clamped in a standard vise is mostly clamp and very little part. Jaw pressure that holds a 100 mm block safely will crush a thin-walled small housing or bow it enough that the top face reads flat while the part is still in the vise and springs back to a curve once released. The measurement is correct and the part is wrong.

We usually move small parts onto fixture plates with dedicated pockets, or onto adhesive film and vacuum chucks when the part has a flat face and no through-holes near the edge. For second operations, cutting soft jaws in place on the machine keeps the locating surfaces concentric with the spindle, which matters more on a Ø8 mm bore than on a Ø80 mm one.

Tabs are the other common answer. A 0.5–1.0 mm tab holds the part during the last passes and gets cut by hand afterward. It costs a finishing step and leaves a witness mark, so we only use it where the profile would otherwise move. On parts with a machined face that must stay cosmetic, tabs are the wrong call and a pocket fixture is the right one.

The judgment is simple. If the part can be held without clamping across the feature you are trying to hold tolerance on, do that. If it cannot, plan the operations so the tight feature is cut while the part still sits on its original stock.

• 1
  Pocket fixturesBest for repeat runs of the same small geometry.
• 2
  Adhesive or vacuumFits flat parts with no edge holes; light depth of cut only.
• 3
  TabsHolds thin profiles, but adds a manual finishing step.

Runout is measured in microns on small tools and it decides tool life. A Ø1 mm carbide end mill with 10 μm of runout puts most of the chip load on one flute. That flute wears first, the cut starts to chatter, and the surface finish goes from Ra 0.8–1.6 μm to visibly torn within a few hundred parts. On a Ø10 mm tool the same 10 μm is a rounding error.

Holders matter more than the machine spec here. Hydraulic and shrink-fit holders keep runout low and hold concentricity through tool changes. A collet chuck that is fine for roughing a bracket will quietly cost you edges on micro work. We check runout on the tool before the first cut on any job with features under Ø2 mm.

Coating selection follows the material, not fashion. Aluminum tends to weld to uncoated and some coated edges, so polished flutes and a light coating work better than a heavy wear coating. Stainless and titanium need the harder coatings and lower surface speed. Plastics generate stringy chips and heat, so we raise feed per tooth and reduce flute count to open the chip room.

Depth of cut is where most programmers overshoot. On a Ø1 mm cutter in aluminum, an axial depth of 0.1–0.3 mm with a light radial stepover keeps deflection predictable. Pushing to 1 mm depth to save a pass usually produces a tapered wall and a broken tool.

• 1
  Check runout before the first cutEspecially below Ø2 mm; 10 μm is the practical ceiling.
• 2
  Match coating to materialAluminum and stainless want different edges.
• 3
  Keep axial depth low0.1–0.3 mm on a Ø1 mm cutter in aluminum.

Aluminum 6061 and 7075 are the forgiving choices for small parts. They cut fast, hold a sharp edge, and tolerate the light depths of cut that micro-tools need. 7075 gives better stiffness on thin ribs. The trade is that aluminum burrs aggressively on small edges, so deburring has to be planned as a step, not as an afterthought.

Stainless 303 and 316 behave differently. They work-harden, so a micro-tool that rubs instead of cutting will dull within a few passes and then start pushing the wall. Feed per tooth has to stay high enough to keep the edge under the surface. On a Ø1 mm cutter that means a careful balance, and it is usually the point where a job needs a test cut before a full run.

Titanium and Inconel are possible on small parts but expensive in tool life. Heat stays at the edge because the chip is too small to carry it away. We reduce surface speed and accept a slower cycle. For prototypes and low volumes that is usually fine. For a 10,000-part run in Inconel, the tooling cost can outweigh the design benefit.

Plastics are the opposite problem. PEEK and POM cut cleanly but hold heat and generate long stringy chips that wrap the tool. We use fewer flutes, higher feed per tooth and air blast instead of flood coolant. PMMA can chip on small edges, so finishing passes stay light.

• 1
  AluminumFast and stable, but plan a deburring step.
• 2
  StainlessWork-hardens; never let the tool rub.
• 3
  Titanium and InconelFeasible, slow, and tool-cost heavy at volume.
• 4
  PlasticsWatch chip wrapping and heat, not rigidity.

Burrs scale with edge geometry, not with part size. A 0.1 mm burr on a 10 mm bracket is proportionally huge and can block assembly or fail a fit check. Hand deburring with a scraper works on a few hundred parts and stops working at volume, because two operators will not produce the same edge.

For repeat runs we prefer controlled methods. Tumbling in ceramic media rounds edges uniformly. Bead blasting cleans the surface and hides light tool marks, though it also softens sharp corners you may have wanted. Electropolishing removes a thin uniform layer and is a good fit for stainless and some titanium parts where edge condition matters more than dimensional change.

Anodizing and plating add thickness. Hardcoat anodizing can build 25–50 μm per surface, which closes a Ø1 mm hole and changes a sliding fit. If a small part carries a tight bore plus a cosmetic finish, machine the bore undersize on purpose and let the finishing step bring it into range, or mask the bore entirely.

Laser marking is often the last operation and it has a floor. Our minimum character height is 1.5 mm, so a serial number on a 6 mm face may not fit. Plan the marking area before the geometry is frozen, not after.

• 1
  TumblingUniform edge rounding for repeat runs.
• 2
  Bead blastingCleans surfaces but softens sharp corners.
• 3
  AnodizingBuilds 25–50 μm per surface; mask tight bores.
• 4
  Laser markingMinimum character height 1.5 mm.

Measuring a 0.5 mm feature with calipers is guesswork. The jaw contact area alone can distort a thin wall and give a reading that is off by more than the tolerance. On small parts we move to optical measurement, vision systems and touch probes, and we measure at a controlled temperature because a 20 mm aluminum part moves several microns between a warm shop and a cold inspection room.

For features under Ø2 mm, contact measurement is often the wrong tool. Optical comparators and vision systems read the edge without touching it, which matters when the wall deflects under a few grams of probe force. CMM touch probing still has a place on bores and datums where you need a hard number, but the probe tip diameter sets the smallest feature it can honestly report.

Inspection planning follows the drawing. Datums first, then the features that stack into the assembly. A tight tolerance on a feature that does not locate anything is a cost with no return, and on small parts that cost shows up fast because the feature may need a separate setup to reach.

We inspect 100% of parts before shipment, with raw material checks, in-process monitoring and a final inspection. Reports are available on request. The point is not the paperwork. It is that a 0.02 mm deviation on a 10 mm part is a 0.2% error, and it can still stop a mechanism from moving.

• 1
  Optical firstNon-contact reads avoid deflecting thin walls.
• 2
  Temperature controlA 20 mm aluminum part drifts microns with shop temperature.
• 3
  Datums before featuresMeasure what locates the part in the assembly.