Where to Use a CNC Machine

• 1
  Where to Use a CNC Machine: Start With Part Geometry
• 2
  Tolerance and Surface Finish Decide the Process
• 3
  Material Behavior Changes the Answer
• 4
  Volume: From One Prototype to 10,000+ Parts
• 5
  Where a CNC Machine Is the Wrong Choice
• 6
  Process Fit by Part Characteristic

The first question is not the material or the quantity. It is whether the part has features that only a rotating cutter can reach. A pocket with a radius at the bottom, a thread that must hold a load, a bore that has to line up with another bore across the part — these are subtractive features. You cannot mold a sharp internal corner, and you cannot print a thread that survives torque. That is where a CNC machine earns its place.

Look at the drawing and count how many directions the tool must approach from. A flat plate with through-holes is a one-setup job on a three-axis mill. A housing with features on four faces needs either multiple setups or a four-axis machine with a rotary table. A part with undercuts, deep cavities, or blended surfaces that wrap around the body usually needs simultaneous five-axis motion, because the tool has to tilt to stay clear of the wall.

Geometry also sets the floor on feature size. On a 4,000 mm gantry we can hold ±0.005 mm on a well-supported feature, but a 0.5 mm wide slot in a thin wall will chatter no matter how good the machine is. When a feature is smaller than roughly three times the tool diameter in depth, tool deflection becomes the limiting factor, not the control.

So before asking for a quote, list the critical features and their approach directions. If every feature points one way, three-axis work is fast and cheap. If they point six ways, that is exactly where a CNC machine belongs, and five-axis will cut the setup count and the stack-up error that comes with it.

• 1
  One approach directionThree-axis mill, single setup, lowest cost
• 2
  Two to four sidesFour-axis or multiple three-axis setups
• 3
  Wrapped or undercut surfacesSimultaneous five-axis, tool tilts to clear the wall
• 4
  Deep narrow slotsTool deflection limits accuracy before the control does

Tolerance is the second filter. If a dimension has to sit inside ±0.05 mm, most processes can get there with enough care. Below ±0.01 mm the list shortens fast, and below ±0.005 mm you are choosing between grinding, lapping, and a rigid CNC setup with temperature control. Our five-axis cells hold ±0.005 mm on aluminum and steel when the part is fixtured properly and the cut is not interrupted.

Surface finish runs in parallel. As-machined 6061 comes off at Ra 1.6–3.2 μm with a normal face mill. If the drawing calls for Ra 0.8–1.6 μm, that means a finer stepover, a sharper insert, and a slower feed on the finishing pass. For Ra 0.2–0.8 μm, the finishing pass is only part of the answer; the part usually needs lapping or polishing after machining, and some geometries cannot be reached by a polishing tool at all.

There is a cost curve here that engineers should see before they release a drawing. Tightening one bore from ±0.05 mm to ±0.005 mm may double the inspection time on that feature and require a separate finishing operation. Tightening a non-critical clearance hole buys nothing. Mark only the dimensions that carry function: bearing seats, seal grooves, locating pins, mating faces.

One more boundary. Tolerance is a property of the whole system, not the spindle. Fixture rigidity, material stress, coolant, and thermal drift all move the number. A part that measures in tolerance on a warm machine can drift out of it after four hours of cutting if the setup is not stable.

• 1
  ±0.05 mmRoutine on most materials with standard fixturing
• 2
  ±0.01 mmNeeds sharp tooling, stable setup, in-process checks
• 3
  ±0.005 mmFive-axis or grinder, temperature control, 100% inspection
• 4
  Ra 0.2–0.8 μmFine finishing plus lapping or polishing on reachable surfaces

Aluminum 6061-T6 and 7075 cut cleanly and hold tight tolerance, which makes them the default for prototype housings and brackets. Copper and brass machine well but move more with heat, so a long finishing pass can pull a thin wall out of tolerance. Stainless 304 work-hardens under a dull cutter, so the feed has to stay heavy enough to cut under the hardened skin instead of rubbing it.

Titanium and Inconel sit at the other end. TC4 (Ti-6Al-4V) and Inconel generate high cutting temperatures because they conduct heat poorly, so the tool edge takes the load. Feed rates drop by roughly half compared with steel, tool life shortens, and the machine has to be rigid enough to avoid chatter at low speed. These are the jobs where five-axis pays for itself, because fewer setups mean fewer chances to scrap an expensive blank.

Plastics behave differently again. POM and ABS cut fast but melt if the chip is not cleared, so air blast matters more than coolant. PEEK and carbon fibre are abrasive and will wear a carbide edge faster than aluminum. Delrin and HDPE flex under clamping pressure, so light fixturing and sharp tooling matter more than machine size.

The material also sets the finishing menu. Anodizing is standard for aluminum, black oxide for steel, electroless nickel for wear surfaces. If the part will be anodized after machining, the mask line and the thread allowance need to be planned before the first cut, not after.

• 1
  Aluminum 6061 / 7075Fast, stable, tight tolerance, easy to anodize
• 2
  Stainless 304 / 316LWork-hardens; keep the feed heavy and the edge sharp
• 3
  Titanium TC4 / InconelHalf the steel feed rate, high heat, rigid setup required
• 4
  POM / PEEK / carbon fibreChip clearing and abrasive wear drive tool choice

CNC has no tooling cost. That single fact decides most volume questions. One part and ten thousand parts use the same program; only the fixture and the cycle time change. There is no mold to cut, no die to harden, no minimum order quantity to hit. We run from a single prototype to 10,000+ part runs on the same machines.

At the low end, from one to about fifty parts, fixtures are simple vises and soft jaws. Setup time dominates the price, so keeping the part to fewer setups saves more than shaving cycle time. At the middle, from a few hundred to a few thousand parts, dedicated fixtures and a bar feeder on the lathe side cut the per-part cost sharply. Above that, the question becomes whether another process takes over.

Die casting and vacuum casting beat CNC on unit cost once the volume is high enough to amortize the tool. Aluminum die casting makes sense somewhere above a few thousand parts per year when wall thickness is uniform and tolerance is looser than ±0.1 mm. Below that line, the tooling cost never pays back. CNC stays cheaper because there is nothing to amortize.

The crossover is not a fixed number. It depends on part size, tolerance, and how often the design changes. For a product still in revision, CNC is almost always the right answer because a design change costs a program edit, not a new tool.

• 1
  1–50 partsSimple fixturing, setup time dominates the cost
• 2
  50–2,000 partsDedicated fixtures and bar feeders cut unit cost
• 3
  Above a few thousand per yearCompare against die casting once tooling amortizes
• 4
  Design still changingStay on CNC; a revision is a program edit, not a new mold

Thin sheet is the clearest case. A 1.5 mm aluminum panel with flanges and louvers is a sheet metal job. Routing it from solid plate wastes material and time, and the flatness will be worse, not better. Laser cutting and bending get there faster and cheaper. The same logic applies to any part whose thickness is small relative to its footprint.

Large hollow shells are another. A pump housing with thin, uniform walls and no tight features is a casting or molding job. Machining it from a solid billet removes 80 percent of the material as chips, and the internal stress released along the way can warp the part after the final pass. If the wall is under 2 mm and the tolerance is ±0.2 mm, casting wins.

Parts with no functional surfaces and a textured look belong to 3D printing. A display model, a jig that only has to hold a sensor in place, a one-off cover with no mating face — printing is faster and needs no fixture. CNC becomes the right answer the moment a dimension carries load or a surface has to seal.

There is also a hard limit on size and access. A deep internal cavity behind a small opening cannot be reached by any standard cutter, no matter how many axes the machine has. In those cases the design has to change, or the part has to be split and assembled. Recognizing that early saves a redesign later.

• 1
  Thin sheet with flangesSheet metal fabrication, not milling from plate
• 2
  Thin-wall hollow shellCasting or molding once tolerance is loose and volume is real
• 3
  No functional surface3D printing is faster and needs no fixture
• 4
  Unreachable internal cavityRedesign or split the part; no cutter can reach it