CNC Machining Manual: How the Machine Turns a Drawing Into a Part

• 1
  Key takeaways
• 2
  What a CNC machining manual actually controls
• 3
  From CAD to G-code: where tolerance is decided
• 4
  Workholding and datums: the setup sheet
• 5
  Roughing, finishing and the limits of the cut
• 6
  Materials, tool wear and why the same alloy behaves differently
• 7
  Where machining stops and another process starts
• 8
  What to put on the drawing so the shop gets it right
• 9
  Feature-by-feature machinability check

A CNC machine does not read a drawing. It reads a sequence of coordinates, feed rates and spindle speeds that a programmer derived from the drawing. That gap is where most production problems start. The drawing says Ø 25 mm ± 0.02 mm. The program says move to X 12.5, Y 0, cut a helix down 18 mm at 1,200 mm/min. Between those two statements sit tool deflection, thermal growth and the stiffness of the setup.

So a useful CNC machining manual is not a list of buttons. It is a set of rules that connect geometry to machine behavior. Three groups of rules matter most on the floor: how the part is held, how the zero point is established, and how the tool enters and leaves the material. Get those right and tolerance follows. Get them wrong and no amount of spindle speed will save the job.

GreatLight runs 127 high-precision CNC machines across three plants in Dongguan and Singapore, including 16 simultaneous 5-axis machining centers. On that floor, the programmers spend more time on the setup sheet than on the tool path. The tool path is largely automated now. The decision about which face to hold, and which face to cut first, is still human.

One more thing before the mechanics. Machining is subtractive, so every feature must be reachable by a rotating tool that comes from outside the part. If you cannot draw a straight line from the tool tip to the feature without hitting the part, the feature needs a different process, a different orientation, or a design change. Keep that test in mind through the rest of this page.

The programmer starts with a solid model and chooses a stock size, usually 1–3 mm oversize on each face. That extra material is not waste. It gives the roughing tool something to bite and it absorbs the distortion that comes from releasing internal stress in the raw bar. For aluminium plate, we often see 0.1–0.3 mm of movement after the first heavy pass. The 2 mm allowance covers it.

Next comes tool selection. A 12 mm carbide end mill removes material fast but leaves a corner radius of 6 mm. If the drawing calls for a 3 mm internal corner, someone has to come back with a smaller tool, and small tools deflect. A 3 mm end mill at 3× diameter depth in 6061 aluminium will push off by 0.02–0.05 mm unless the depth of cut is reduced. That is the whole tolerance budget on a ±0.005 mm callout.

Feeds and speeds come from the material, not from habit. In 6061-T6, a 12 mm three-flute carbide cutter runs well around 8,000 rpm and 2,500 mm/min with a 6 mm axial depth. In 316L stainless, the same cutter drops to roughly 1,800 rpm and 400 mm/min. Inconel is slower again. These numbers are starting points. The operator adjusts by sound and chip shape, because the same nominal alloy can behave differently between heats.

Finally the post-processor converts the CAM tool path into machine-specific G-code. This is where a good CNC machining manual earns its keep: the post must match the control, the rotary table orientation and the tool-length offsets actually loaded in the machine. A post that is one revision out of date produces a crash, not a part.

The setup sheet defines the zero point. In a 3-axis vise job, that is usually the top-left corner of the stock with Z zero on the top face. In 5-axis work, it is the center of the rotary table, and every offset is measured from there. When the datum does not match the drawing's datum, dimensions stack up in the wrong direction and the part fails inspection even though every cut was correct.

Workholding stiffness matters more than most designers expect. A part held in a vise with 30 mm of unsupported material above the jaws will chatter. Chatter shows up as a poor surface finish and, worse, as a dimension that drifts along the wall. Reducing the stick-out, adding a support jack, or switching to a dovetail fixture solves it. On thin-walled parts, we often machine a soft-jaw pocket that matches the part profile, so the clamping force spreads over a larger area.

For parts above 500 mm, vacuum chucks and modular fixturing take over from vises. GreatLight machines up to 4,000 mm, with travels of 4,000 × 400 × 150 mm on the largest beds. At that size, thermal expansion is a real term in the tolerance equation. A 1,000 mm aluminium part grows about 0.023 mm per °C. A shop floor that swings 4 °C between morning and afternoon moves the part more than a ±0.005 mm callout allows, which is why temperature-controlled cells exist.

The practical rule: decide the datum before you decide the tool path, and never re-clamp a part for a finishing pass unless you have to. Every re-clamp resets the error budget.

Roughing removes 70–90 percent of the stock with the largest rigid tool available. Leave 0.3–0.5 mm of radial stock for finishing on most steels, 0.2–0.3 mm on aluminium. Any less and the finishing tool hits the hardened skin left by the roughing pass. Any more and the finishing tool takes a heavy load that deflects it away from the wall.

Finishing is where surface finish is set. Ra 3.2 μm is a normal as-machined result. Ra 1.6 μm needs a sharper tool, a smaller stepover and a stable setup. Ra 0.8 μm or better usually means a finishing pass at low feed with a wiper insert or a small stepover on a ball nose. GreatLight holds Ra 0.2–0.8 μm on finish-critical faces, but those faces cost time, and time is the price of the part.

Then there are the features that resist milling. A pocket deeper than 4× its width needs a long, thin tool that deflects. An internal corner sharper than the smallest available cutter radius cannot be cut at all; it becomes a wire EDM or a sinker EDM job. A floor thinner than 1 mm will ring and dish under cutting force. None of these are impossible. They are simply more expensive than the design usually assumes.

Drilled holes follow the same logic. A hole 10× diameter deep in stainless will wander unless it is spot-drilled and pecked. A cross-hole that breaks into another bore needs deburring from both sides, which means an extra setup or a hand operation. Add those to the routing early, not after the first article.

Aluminium 6061 and 7075 cut freely but differ in stability. 7075 holds a better surface on thin walls; 6061 welds to the cutter more easily and needs a sharper edge and more coolant. Plastics are the opposite problem: POM and PEEK cut cleanly but move after machining, so a ± 0.02 mm callout on a 100 mm PEEK part is realistic only after a stress-relief step.

Stainless 304 and 316L work-harden. If the tool rubs instead of cutting, the surface gets harder and the next pass wears the tool faster. The fix is constant feed, no dwell, and a fresh edge. Titanium Ti-6Al-4V adds heat to the problem. Cutting temperatures reach 1,000 °C at the edge, so coolant delivery and tool coating matter as much as speed.

Tool wear is a slow drift, not a sudden failure. A carbide insert run past its wear land will push the dimension by 0.01–0.03 mm before the operator hears anything. That is why in-process measurement matters on tight jobs. GreatLight runs raw material checks, in-process monitoring and final inspection on every order, with reports on request, and holds a 99.99 percent qualification rate on shipped parts.

For any material, the safest design move is to specify the alloy and temper, not just the family. 6061-T6 and 6061-O machine nothing alike. The same applies to 17-4PH: condition H900 and condition A differ in hardness by a factor of three.

Machining is unbeatable for tight tolerance on a small number of parts and for features that need one continuous surface. It is a poor choice for a part with 40 identical small holes in a thin plate, where laser cutting or stamping wins on cycle time. It is also a poor choice when the geometry is mostly hollow with 2 mm walls, which is a die casting or sheet metal job.

Volume changes the answer. A single prototype in 6061 costs a setup and a few hours of spindle time. At 10,000 parts a year, casting plus a light finishing cut usually beats milling from solid. The crossover depends on feature count and tolerance, not on weight alone. GreatLight runs from one prototype to 10,000+ part runs with no minimum order quantity, so we see both ends of that curve.

Additive processes compete in a narrow band: internal channels that no cutter can reach, lattice structures, and parts where the geometry is fixed but the volume is low. Where a machined surface is still required, the printed blank is finished on a 3-axis or 5-axis machine, and the same tolerance rules apply to the finished faces.

The engineering point is simple. Choose the process by the feature that is hardest to make, not by the feature that covers the most area.

A drawing that machines cleanly has three things: a clear datum scheme, a tolerance that matches the function, and a note about edges. Default tolerances of ± 0.1 mm on a part that only needs ± 0.25 mm add cost for no benefit. Conversely, a ± 0.01 mm callout on a face that will be painted is money spent on nothing.

Call out the critical faces. If two bores must share an axis, say so with a geometric tolerance rather than a stack of dimensions. If a face is a sealing surface, give the flatness and the finish. Everything else can stay general. This is the single biggest cost lever a designer holds.

Include the material condition, the finish, and whether the part will be anodized before or after any press-fit operation. Anodizing adds 5–25 μm per surface depending on the type, which matters on a Ø 10 H7 bore. Laser marking needs a minimum character height of 1.5 mm to stay legible after coating.

Finally, send the 3D model with the drawing. The model removes ambiguity about blends and corner radii; the drawing carries the tolerance intent. Shops that get both produce fewer first-article surprises. GreatLight returns a free DFM analysis with the quotation within 12 hours, and production can start within 24 hours after approval.