Manual CNC Machining Basics: How the Process Actually Works

• 1
  What manual cnc machining actually removes
• 2
  How many axes a part really needs
• 3
  Tolerances that hold on the shop floor
• 4
  Design rules that keep quotes low
• 5
  Materials, finishing and what happens after cutting
• 6
  Which setup fits your part

CNC machining is subtractive. A rotating cutter removes material from a solid block until the remaining geometry matches the CAD model. Nothing is added, so every pocket, slot and thread has to be reachable by a tool that spins on a fixed axis. That single constraint explains most of the cost differences between two parts that look similar on a drawing.

The cutter is not rigid. It bends under cutting force, and the amount it bends depends on how far it hangs out of the holder. A Ø10 mm end mill held 40 mm from the collet behaves very differently from the same tool held 80 mm out. Long reach means light depth of cut, slower feed, and more passes. That is why a deep narrow pocket costs more than a wide shallow one of the same volume.

Heat matters too. Aluminium 6061 conducts heat away quickly and cuts clean at high spindle speeds. Titanium TC4 and Inconel keep heat at the cutting edge, so surface speed drops by roughly a factor of five to ten and tool wear climbs. The same feature that takes four minutes in aluminium can take thirty in Inconel. Design reviews should treat material choice as a cost decision, not just a strength decision.

Chip evacuation is the quiet failure mode. If chips pack into a pocket, the tool recuts them, which raises cutting force and ruins the floor finish. Deep pockets with small corner radii are the classic case. Adding a corner radius that matches a standard tool, or opening the pocket floor with a draft, often removes an entire roughing pass from the program.

• 1
  Reach drives costTool length-to-diameter ratio above 6:1 needs reduced feeds and extra passes.
• 2
  Material sets speedAluminium cuts fast; titanium and nickel alloys cut five to ten times slower.
• 3
  Chips must escapeDeep pockets with tight corners trap chips and damage finish.

A 3-axis machine moves the table in X, Y and Z while the tool stays vertical. It is the cheapest way to cut flat plates, brackets, housings with open faces, and anything that can be reached from one direction. If a part can be made in two or three setups on a 3-axis machine, that is usually the right call. Extra axes only pay for themselves when they remove setups or reach geometry that no fixturing can expose.

A 4-axis machine adds rotation about one horizontal axis, normally a rotary table. This suits parts with features on several sides of a cylinder or a prismatic block: shaft flats, cross-drilled holes, cam profiles. The part turns instead of being re-fixtured, so hole-to-hole position stays tight. We run 12 four-axis mills alongside a Ø400 mm rotary table for work that needs indexing rather than full contouring.

A 5-axis machine moves the tool or the table on two rotational axes at once, and the two axes move together during the cut. This lets a short, stiff tool reach undercuts, blend sculpted surfaces, and drill at compound angles without re-clamping. Simultaneous five-axis work is what makes impellers, medical bone plates and thin-walled aerospace ribs practical. We run 16 simultaneous 5-axis machining centers for exactly this class of part.

The trade-off is programming and verification time. A 5-axis toolpath has to be checked for gouges and collisions along the whole move, not just at the endpoints. For a simple part with five holes on five faces, a 4-axis setup or two 3-axis setups will be cheaper and just as accurate. Choose 5-axis when the geometry demands it, not because the machine is impressive.

• 1
  3-axisFlat plates, open pockets, parts reachable from a few directions.
• 2
  4-axisCylindrical or prismatic parts needing indexed features on several faces.
• 3
  5-axisUndercuts, sculpted surfaces, compound-angle holes, thin walls.

A tolerance is a statement about process capability, not a wish. On a rigid setup in aluminium or brass, ±0.005 mm is achievable on bores and mating faces. On a long slender part, or in titanium, the same callout may be impossible to hold repeatably because the part moves as material is removed. The number on the drawing has to match the stiffness of the part and the material it is cut from.

Thermal drift is the other limit. A machine that has been running for four hours is not at the same temperature as one that just started. For tight work we let the machine idle to thermal equilibrium and check the first article before running the batch. This is normal practice, not a special service, and it is the difference between a tolerance that holds on part one and part two hundred.

Surface finish follows the same logic. As-machined finish sits around Ra 1.6–3.2 μm. Careful toolpath and sharp tooling get to Ra 0.8–1.6 μm. Below that, Ra 0.2–0.8 μm, you are usually looking at a secondary operation such as fine tumbling or polishing, because the required edge quality cannot come from a single pass. Specify finish where it functions, not across the whole part.

Inspection closes the loop. We check raw material on arrival, monitor in-process dimensions, and inspect 100% before shipment, with reports on request. A tolerance that nobody measures is not a tolerance. If a dimension is critical to function, say so on the drawing so it gets measured and recorded rather than spot-checked.

• 1
  ±0.005 mmRealistic on rigid setups in aluminium, brass and free-machining steel.
• 2
  Thin walls moveSlender parts and titanium need looser tolerances or added support.
• 3
  Finish is a stepRa 0.2–0.8 μm usually needs a secondary finishing operation.

Internal corners cannot be square. A rotating cutter always leaves the radius of the tool at the corner, so a pocket drawn with a sharp corner will be quoted either with a small tool and many passes, or with an EDM operation. Specify a corner radius at least equal to the depth of the pocket divided by six, and pick a radius that matches a standard cutter diameter. That one change often cuts cycle time noticeably.

Threads and holes have depth limits. A tapped hole deeper than about three times its diameter needs a longer tap and a more careful peck routine, and blind holes need clearance at the bottom for the tap lead. Standard drill point angles leave a cone at the bottom of a blind hole, so a hole drawn to a flat depth may need a flat-bottom cutter and a second operation. Call out thread depth, not just hole depth.

Wall thickness matters more than most drawings admit. A wall thinner than about 0.8 mm in aluminium will deflect under cutting force and chatter, and the finish will show it. If the design needs a thin wall, add a temporary rib or leave stock that gets removed in a finishing pass. For parts that must be light and thin, five-axis contouring with a small stepover holds the wall better than a 3-axis approach.

Text and engraving needs room. Laser marking holds a minimum character height of 1.5 mm, and engraved text cut with a cutter needs wider strokes. Put part numbers on a flat face rather than a curved one, and keep marking away from sealing surfaces and bearing fits. A part number engraved in the wrong place can turn a good part into scrap.

• 1
  Corner radiusMatch a standard cutter; sharp internal corners need EDM.
• 2
  Thread depthBlind holes need tap lead clearance; call out thread depth.
• 3
  Thin wallsBelow ~0.8 mm in aluminium, expect deflection and chatter.

Material choice sets the whole cost structure. Aluminium 6061, 6061-T6, 2024, 5052, 6063, 6082, 7075 and ADC12 all machine well and cover most brackets, housings and heat sinks. Stainless 303 and 304 are common for shafts and fittings, while 17-4PH and 316L appear in medical and marine work. Tool steel, 4140 and 4340 handle higher loads. Titanium TC4, Inconel and magnesium AZ31B are cut here too, at slower rates and higher cost.

Plastics behave differently again. POM and PA cut cleanly, PC and PMMA can craze or chip at the edges, and PEEK and carbon fibre wear tooling quickly. Carbon fibre in particular needs diamond-coated cutters and dust control. For prototypes in these materials, the same geometry that works in aluminium may need different feeds, different fixturing and a different finishing step.

Finishing is where the part becomes a product. Anodizing in clear, colour, hardcoat or conductive form changes both appearance and wear resistance. Electroless nickel, zinc, silver and gold plating cover electrical and corrosion needs. Powder coating and black oxide handle larger frames. Bead blasting, tumbling, brushing and polishing set the cosmetic grade. Laser marking and engraving add traceability.

The sequence matters. A part that is anodized after tapping will have a coating build-up in the threads unless masking is planned. A part that is bead blasted after a tight bore may lose the bore tolerance. Good drawings state the finishing sequence and which surfaces are masked. We build that sequence into the process plan rather than discovering it at the last step.

• 1
  Aluminium family6061, 7075, 2024, 5052, 6082, ADC12 cover most enclosures and brackets.
• 2
  Stainless and steel303, 304, 316L, 17-4PH, 4140, 4340 for load and corrosion.
• 3
  Finish orderAnodize after tapping builds thickness in threads unless masked.