CNC Processing Gallery: What the Parts Actually Tell You

• 1
  Reading a CNC processing gallery correctly
• 2
  How part geometry maps to 3-axis, 4-axis and 5-axis work
• 3
  Why the same part machines differently in aluminum and titanium
• 4
  Surface finish is a process decision, not a cosmetic one
• 5
  When a machined part is the wrong choice
• 6
  Process route by geometry and volume

A CNC processing gallery is a record of what a shop actually cut, not a catalog of pretty renders. The useful ones show the part, the material, the tolerance band and the finish. When we publish a part, the question we answer is simple: which machine and which setup produced this, and why.

Most galleries fail on one point. They show the finished part but hide the fixture. Turn a complex aluminum housing over and the second operation is where the real difficulty lives. Datum shift, clamp marks, chatter near thin walls. A gallery that omits the setup notes tells you very little about whether your own part is a fit.

So the first habit is to read the geometry, not the photograph. Look for undercuts, deep pockets, small internal radii, wall thickness under 1 mm, and cross-holes on different axes. Each of those points to a specific machine configuration and a specific cost driver.

Second habit: read the tolerance callout. A ±0.1 mm bracket and a ±0.005 mm manifold body can look identical in a photo. The machining time, the inspection burden and the scrap risk are not close. A gallery without tolerance data is decoration.

• 1
  Show the setupFixture, workholding and operation count matter more than the render.
• 2
  Show the toleranceA number per critical feature, not a general claim.
• 3
  Show the materialAluminum 6061 and Ti-6Al-4V behave nothing alike on the spindle.

A 3-axis machine moves the tool in X, Y and Z while the part stays fixed. That covers most prismatic parts: plates, brackets, covers, manifolds with features reachable from one or two directions. Setup is simple, fixturing is cheap, and cycle time is predictable. If your part is a flat plate with pockets and through-holes, 3-axis is usually the right answer.

A 4-axis machine adds a rotary table, typically Ø400 mm, so the part can index around one axis. Think of a shaft with cross-drilled holes, or a long extrusion with features on four faces. You cut operation one, rotate 90°, cut again. Fewer setups, better position between faces. The limit is that the tool still approaches from one side.

A 5-axis machine moves the tool and the part at the same time, or tilts the spindle. That lets the cutter stay normal to a curved surface and reach under overhangs without re-fixturing. Complex impellers, turbine blades, orthopedic implants and thin curved housings are the classic cases. The trade-off is programming time and a tighter verification loop.

The practical rule we use: if a feature can be reached in two orthogonal setups on a 3-axis machine, do not pay for 5-axis. If reaching it needs three or more setups, or a custom angled fixture, 5-axis usually wins on total cost even though the hourly rate is higher.

• 1
  3-axisPrismatic parts, features reachable from one or two directions.
• 2
  4-axisRotational parts with cross features, long parts on a rotary table.
• 3
  5-axisSculpted surfaces, undercuts, tight position between many faces.

Aluminum 6061 cuts fast. Spindle speeds run high, tools last, and a light finishing pass gives Ra 0.8–1.6 μm without much effort. That is why so many prototype parts in a gallery are aluminum. The failure mode is thin walls. Aluminum deflects under clamping and under cutting force, so a 0.8 mm wall will move unless the fixture supports it.

Stainless 304 and 316 work-harden. If the tool rubs instead of cutting, the surface gets harder and the next pass is worse. The fix is a positive feed per tooth and no dwelling in the cut. 17-4PH in the H900 condition is harder again, and it is common in medical and aerospace work where the material properties are the reason for the part.

Titanium Ti-6Al-4V has low thermal conductivity. Heat goes into the tool edge instead of the chip, so edge life drops fast. Cutting speed comes down, coolant strategy matters, and cycle time goes up roughly two to three times versus aluminum for the same geometry. That cost is a material property, not a shop markup.

Plastics behave differently again. POM and PEEK machine cleanly with sharp tools and air blast, but they expand with heat and can creep under clamp pressure. ABS and PC are softer and prone to burrs. For any plastic part, the tolerance you can hold is looser than the same feature in aluminum.

• 1
  AluminumFast, forgiving, watch thin walls and clamp marks.
• 2
  StainlessWork-hardening; keep the tool biting, never rub.
• 3
  TitaniumHeat sits in the edge; lower speed, shorter tool life.
• 4
  PlasticsThermal growth and burrs set the real tolerance band.

As-machined surfaces land around Ra 1.6–3.2 μm with visible tool marks. That is fine for brackets, fixture plates and internal parts. A high-finish pass brings it to Ra 0.8–1.6 μm and removes most of the marks. Fine finishing, Ra 0.2–0.8 μm, needs a separate light pass with a fresh tool, often a smaller stepover, and it costs time.

Anodizing changes dimensions slightly. Type II clear anodizing adds a thin oxide layer, hardcoat adds more. If you have a ±0.005 mm bore that must stay on size, mask it or plan the pre-anodize dimension. The same applies to electroless nickel and zinc plating, where the coating thickness sits on every surface unless you mask.

Bead blasting and tumbling even out tool marks and deburr edges. Brushing gives a directional grain. Polishing pushes toward a mirror finish but can round a sharp edge you wanted to keep. Tell us which edges are functional and which are cosmetic; that single note saves a rework cycle.

Laser marking is the last step and it is easy to get wrong. Minimum character height is 1.5 mm. Below that, the mark smears and does not read. If your part number or UDI needs to survive sterilization or a wash cycle, say so before marking, because the marking depth and the surface prep change.

• 1
  Function firstSealing faces and bearing bores need the tightest finish.
• 2
  Coating growthAnodize and plating add material; mask critical bores.
• 3
  Marking limits1.5 mm minimum character height for a clean laser mark.

CNC machining wins on accuracy and on geometry that other processes cannot reach. It loses when the part is simple and the volume is high. A plain bracket at 50,000 pieces a year is a die casting or a stamping, not a milling job. The tooling cost is real, but the per-part cost falls far below any subtractive route.

It also loses when the part is mostly hollow with thin uniform walls and no tight features. That shape is a casting or a molding. Machining it means removing most of the stock as chips, and you pay for the material you throw away.

There is a middle ground worth knowing. Die casting plus a light machining pass gives you the cast shape with machined bores and sealing faces. That combination shows up often in automotive and EV work, and it is usually cheaper than cutting the whole part from billet once volumes pass a few thousand.

For one prototype, none of this matters. Cut it from billet, check the fit, and move on. The process decision should follow the volume curve, not the other way around.

• 1
  Pick machiningLow to mid volume, tight tolerance, complex geometry.
• 2
  Pick castingHigh volume, simple shape, generous tolerance.
• 3
  Pick hybridCast body plus machined critical faces at mid-high volume.