Basic Knowledge of CNC Machining for 3D Parts

CNC machining removes material with a rotating cutting tool. A CAM programmer takes your solid model, picks a tool, and generates a toolpath. That path is posted as G-code, which the machine controller reads and executes. Nothing about the geometry changes at this stage. The model is either machinable or it is not, and that is decided by tool access and fixturing, not by software.

The chain usually runs: roughing with a large end mill to clear bulk material, semi-finishing to leave an even stock allowance, then finishing passes that produce the final surface. A 50 mm face mill can remove metal fast but cannot enter a 6 mm corner. A 3 mm ball nose can reach that corner but needs many more passes. This trade-off is the core of basic knowledge in CNC machining, and it shows up directly in cycle time.

For a typical 3D part, we inspect the raw material certificate before cutting, monitor dimensions during the run, and measure the finished part before it ships. Reports are available on request. If a feature cannot be measured with a standard touch probe, say so on the drawing, because that changes how we plan the setup.

A 3-axis machine moves the tool in X, Y, and Z while the part stays fixed. It is the fastest and cheapest option when every machined face can be reached from one or two directions. Plates, brackets, housings with open pockets, and most prismatic parts fall here. Roughly 27 of our machines are 3-axis, which is where simple work should stay.

A 4-axis machine adds rotation around one axis, usually A. That lets you cut features on multiple sides of a shaft-like part without re-clamping. A 12 mm cross-hole in a Ø40 mm shaft is a good 4-axis job. So is a part with a bolt pattern on its end face plus a slot along its length. We run 12 four-axis mills for exactly this class of work.

A 5-axis machine moves the tool and the part at the same time. It reaches undercuts, deep cavities, and compound angles in one setup. Impellers, turbine blades, medical bone plates, and any part with a curved surface that must be cut normal to the toolpath belong here. We have 16 simultaneous 5-axis machining centers and 16 mill-turn centers for parts that need turning and milling in one cycle.

The rule of thumb: if a part needs three or more setups on a 3-axis machine, check whether 5-axis can do it in one. Every extra setup adds fixture cost, stack-up error, and labor. Sometimes 5-axis is cheaper even at a higher hourly rate.

• 1
  Stay 3-axisOpen pockets, flat faces, through-holes, parts under 500 mm with simple access.
• 2
  Move to 4-axisShafts, bushings, and parts with features indexed around one centerline.
• 3
  Move to 5-axisCompound angles, deep undercuts, curved blades, or features on five faces.

Internal corners are cut by a round tool, so they always carry the tool radius. If your model shows a sharp 90° internal corner, the CAM programmer will either leave the radius or burn a small cutter that takes far longer. Specify the largest acceptable corner radius. A 3 mm radius in a pocket is normal; a 0.5 mm radius forces a fragile tool and a slow feed.

Pocket depth matters too. A useful starting point is a depth-to-width ratio of about 4:1 for a standard end mill in aluminum. Beyond that, tool deflection grows, chatter appears, and the finish degrades. If you need a 10 mm wide pocket that is 60 mm deep, expect either a reduced tolerance, a larger radius, or an EDM step that raises cost.

Threads and holes should be called out with a standard size where possible. A 1/4-20 or M6 tapped hole is routine. A non-standard thread pitch requires a custom tap or single-point threading, which adds time. Blind holes should include a thread depth and a drill depth, because the tap cannot go to the very bottom of a drilled hole.

Text and logos cut into a surface need to be at least 1.5 mm tall for laser marking, and deeper for engraving. Thin raised lettering under 0.5 mm wide tends to break or blur. If the mark is cosmetic, put it on a flat face that the tool can reach in the finishing pass.

Not every dimension needs the same tolerance. A general tolerance block of ±0.1 mm covers most non-critical features and keeps the part cheap. Reserve tight callouts for the features that actually mate or locate. We hold ±0.005 mm (±0.0002 in) when a drawing requires it, but applying that to a whole part multiplies inspection time and scrap risk.

Surface finish follows the same logic. As-machined at Ra 1.6–3.2 μm is fine for brackets and internal parts. Ra 0.8–1.6 μm is a normal fine finish for sealing faces and sliding surfaces. Ra 0.2–0.8 μm requires slower feeds, a sharper tool, and often a second operation. Tell us which faces need it rather than calling out the whole part.

Material choice interacts with all of this. Aluminum 6061 and 7075 cut cleanly and hold tight tolerances well. Stainless 316 and 17-4PH work-harden, so light passes and rigid setups are required. Titanium TC4 and Inconel move more under heat, which means rough, cool, and finish as separate steps. Plastics like POM and PEEK machine fast but deflect, so thin walls need support.

A short note on the drawing: mark the datum faces. If the part is located from a face that we cannot clamp on, the first operation will not match the intent. Two minutes of datum planning on your side saves a fixture redesign on ours.