How to CNC Machine Working: From CAD File to Finished Part

• 1
  Key takeaways
• 2
  How to CNC Machine Working Starts with the CAD File
• 3
  CAM Programming: Turning Geometry into G-code
• 4
  Workholding and Setup Decide the Tolerance
• 5
  Tool Selection and Cutting Parameters
• 6
  First-Article Check and In-Process Monitoring
• 7
  When CNC Machining Is the Wrong Process
• 8
  Step by Step: How to CNC Machine Working on the Shop Floor
• 9
  Which Process Fits: Quick Comparison

The chain starts with a 3D solid, not a drawing. A STEP or IGES file carries the geometry; a PDF drawing carries the tolerances, datum scheme and finish callouts. Both are needed. A model alone cannot say whether a bore is Ø10 H7 or a clearance hole, and a drawing alone leaves CAM software with nothing to calculate toolpaths on.

Before programming, the model gets checked for manufacturability. Sharp internal corners become radius calls based on the smallest cutter that can reach them. A 6 mm end mill leaves roughly a 3 mm corner radius, so any internal corner drawn tighter than that needs EDM or a smaller tool with a longer cycle time. Depth-to-diameter ratios above about 4:1 for end mills and 8:1 for drills are where tool deflection and chip evacuation start to matter.

Wall thickness and floor thickness get the same treatment. Thin floors vibrate under cutting load. Aluminum walls at 0.8 mm and stainless walls at 1.5 mm are workable, but they need light radial engagement and a supporting fixture. If a wall is thinner than the tolerance on the drawing, we flag it before quoting rather than after the first part is cut.

At GreatLight we run this DFM pass as part of quoting. A quotation and free DFM analysis come back within 12 hours, so the changes are still cheap to make. The output of this stage is a model that CAM can trust plus a list of features that need special attention.

CAM software reads the solid and outputs G-code, the instruction list the controller executes. Two path families cover most work. Roughing removes the bulk of material with large stepdowns and fast feed rates. Finishing follows with small radial steps to hit the surface callout, typically Ra 0.8–1.6 μm on a well-supported wall.

Toolpath strategy drives cycle time more than spindle speed does. Trochoidal or dynamic roughing keeps radial engagement low and axial depth high, which spreads heat into the chip instead of the tool. On 6061-T6 this often lets a 10 mm carbide end mill run at 0.08–0.12 mm/tooth with a 1×D axial depth, where a conventional path would need three passes to reach the same depth.

Stock left for finishing is normally 0.3–0.5 mm on walls and 0.2 mm on floors. Too little and the finish pass rubs; too much and the cutter deflects. On thin parts, a spring pass with zero radial offset cleans up the wall without adding load.

Simulation comes before the machine. The CAM file gets checked for rapid collisions, holder interference and axis travel limits. Our largest travel is 4,000 × 400 × 150 mm, our medium machines run 750 × 1,150 × 550 mm and 600 × 600 × 600 mm, and the compact cells run 500 × 500 × 450 mm. A program that fits the model but not the machine is caught here, not at the spindle.

A vise, a 3-jaw chuck and a vacuum plate all have a stiffness limit. The part sees cutting force in the direction of travel, and wherever the fixture is soft, the part moves. That movement shows up as chatter marks, out-of-round bores and a flatness number that drifts between the first and last part of a run.

For prismatic parts, a machine vise on parallels with 2–3 mm of material gripped works for most roughing. For a second operation on a finished face, soft jaws bored to the part diameter give better repeatability than hard jaws. For thin plates, a vacuum table with a dedicated gasket layout spreads the load across the whole face.

Datum selection matters as much as the clamp. Three faces, two holes, or a face plus two edges give a repeatable origin. Single-point datums on a curved surface do not. When the drawing calls for a positional tolerance of 0.02 mm, the fixture needs to hold the part within roughly a third of that during cutting, so 0.006–0.007 mm of fixture-induced movement is the budget.

Round parts go to a lathe or a mill-turn center. Our mill-turn cells handle turned features and milling in one setup, which removes the re-datum error that a two-setup process introduces. Shafts with a length-to-diameter ratio above 4:1 often need a tailstock or a steady rest, otherwise the part deflects away from the tool.

Carbide is the default for aluminum, steel, stainless and titanium. Coatings change the heat picture: TiAlN and AlTiN suit dry or near-dry steel and stainless cutting, while uncoated or DLC-coated tools suit aluminum because aluminum tends to stick to hard coatings. Diamond-coated tools are reserved for abrasive non-ferrous work and graphite.

As a starting point on 6061-T6 aluminum, a 10 mm 3-flute carbide end mill runs at roughly 12,000–18,000 rpm, 0.08–0.12 mm/tooth and a 1×D axial depth. On 304 stainless with the same diameter, expect 2,500–4,000 rpm, 0.03–0.05 mm/tooth and a 0.3–0.5×D axial depth. On Ti-6Al-4V, reduce surface speed further and keep coolant flooding the cut, because titanium conducts heat poorly and the edge will burn without it.

Coolant choice is not cosmetic. Flood coolant controls heat in deep pockets and stainless. High-pressure through-tool coolant is what makes a 10×D drill possible without pecking every 0.5 mm. Air blast handles aluminum where thermal shock is not a concern. Mist is the weakest option and we avoid it on anything with a tight tolerance.

Tool life is tracked, not guessed. A tool change interval is set from the material removal volume, and the operator logs when the edge starts to pull. One dull tool on a finishing pass can turn a ±0.005 mm bore into a scrapped part, so finishing tools are changed on schedule, not on noise.

The first part off the machine is measured in full. Calipers are not enough for a tolerance of ±0.005 mm. A coordinate measuring machine, micrometers or bore gauges with the right resolution are the tools for the job. The report compares every dimension on the print, not just the ones that look risky.

If the first article is in tolerance, the run starts and the process is monitored. Operators check critical features at set intervals, usually every 5 to 20 parts depending on the feature and the tool wear rate. Dimensions that drift in one direction indicate thermal growth or tool wear; dimensions that jump indicate a fixture or chip problem.

Environmental drift is real. A shop floor that swings 5 °C over a shift will move a 300 mm aluminum part by more than the tolerance on a tight print. Temperature-controlled inspection rooms exist for that reason, and final measurement is done after the part has cooled to room temperature.

At GreatLight, inspection covers raw material check, in-process monitoring and final inspection, with 100% inspection before shipment and reports on request. Our qualification rate is 99.99%. That number is only possible because the checks happen during the run, not after it.

CNC is a subtraction process, and subtraction has a cost curve. For one to a few hundred parts in metal, it is usually the right answer. Past a few thousand identical plastic parts, injection molding takes over because the tooling cost gets divided across the volume. Die casting does the same for metal housings at high volume.

Geometry sets the second limit. Deep, narrow slots, sharp internal corners tighter than about 1 mm, and features on the far side of a long bore all need either a special tool or a second process. Electrical discharge machining can cut a sharp internal corner, but it is slower and often needs a separate electrode.

Material sets the third. Soft rubber and silicone parts do not machine cleanly; they smear and tear. Very thin, flexible sheet metal is usually better laser-cut and formed. And parts that need internal channels with no straight-line access are candidates for 3D printing rather than milling.

If your part is in the gray zone, send the model. We will tell you whether CNC, sheet metal, casting or 3D printing fits better, and the DFM analysis is free. There is no minimum order quantity, so a single prototype and a 10,000+ part run go through the same review.