CNC Processing Guide: A Step by Step Walkthrough

• 1
  Key takeaways
• 2
  What CNC Processing Actually Is
• 3
  Prepare the CAD File and Drawing
• 4
  DFM Review and Quotation
• 5
  Material Choice Sets the Cutting Window
• 6
  Setup, Workholding, and Datum Transfer
• 7
  Tolerances and Surface Finish in Practice
• 8
  Common Mistakes That Scrap Parts
• 9
  The 7 Steps of CNC Processing
• 10
  Choosing the Right Process for the Feature

CNC processing is subtractive manufacturing driven by a program. A CAD model becomes toolpaths, toolpaths become G-code, and the machine moves a spinning cutter through a block of metal or plastic until the shape matches the model. Nothing is molded or cast. Material is removed.

The word covers turning, milling, drilling, and the multi-axis combinations of all three. On a 3-axis mill the tool approaches from one direction. On a 5-axis center the tool tilts, so undercuts, angled holes, and deep pockets open up without re-fixturing.

This CNC processing guide is written from the shop side. Whether you send one prototype or a 10,000-part run, the sequence is the same: review, quote, setup, cut, inspect, finish, ship. The variables change, the order does not.

• 1
  Subtractive, not additiveStock is removed. Design for tool access, not for layer support.
• 2
  Program-drivenEvery pass is repeatable. The first good part defines the rest.
• 3
  One process, many machinesTurning, milling, and mill-turn cover different geometry families.

Send a STEP or Parasolid solid plus a 2D PDF drawing. The solid defines geometry; the drawing defines what must be measured. If a dimension matters, it belongs on the drawing with a tolerance. If it does not, leave it to the general callout.

Thread callouts are a common failure point. Write M6 × 1.0, not "M6 tapped hole". For pipe threads, state the standard. For press fits, give the fit class, not just the nominal diameter.

Set your datums on functional surfaces: a mounting face, a bore centerline, a locating pin. Datums picked off a cosmetic edge force the machinist to guess, and guessing costs time. If you need first-article data, say so at quote stage.

• 1
  Model plus drawingSTEP for geometry, PDF for tolerances and notes.
• 2
  Tolerance only where neededBlanket ±0.1 mm on every dimension inflates the price.
• 3
  Name the material grade6061-T6 and 6061-O machine very differently.

A DFM review checks whether the part can be cut with the tools you have paid for. Thin walls under 0.8 mm in aluminium, pockets deeper than 4× the cutter diameter, and sharp internal corners are the usual flags. None of these are impossible. They change the tool, the cycle time, and sometimes the setup count.

Corner radii should be at least one third of the pocket depth where possible, so the largest practical cutter fits. A 6 mm corner in a 25 mm deep pocket forces a small tool and a long, slow pass. Open the corner to 8 mm and the cycle time drops.

Ask for the quote to list material, finish, tolerance class, and inspection scope separately. That way you can see what a tighter tolerance or a hardcoat anodize actually adds before you commit.

• 1
  Wall thicknessKeep aluminium walls at 0.8 mm or more for stable cutting.
• 2
  Pocket depthBeyond 4× cutter diameter, expect reduced feed and more passes.
• 3
  Corner radiusMatch the radius to the largest cutter that fits the pocket.

Aluminium 6061-T6 is the default for prototypes and brackets: free-cutting, weldable, and cheap to anodize. 7075 gives higher strength for aerospace fittings but machines slower and anodizes darker. 2024 sits between them and is common in aircraft structure.

Stainless 303 is the turning grade. 304 and 316 are tougher, gummier, and prone to work hardening if the tool rubs instead of cuts. Keep the feed per tooth up and the radial engagement down. 17-4PH in the H900 condition will hold ±0.005 mm, but only after stress relief.

Titanium TC4 (Ti-6Al-4V) and Inconel are heat-limited. Cutting speeds drop by roughly a factor of four against aluminium, and tool life is measured in minutes. If the part does not need the temperature or strength, do not specify it.

• 1
  Aluminium first6061-T6 covers most fixtures, housings, and brackets.
• 2
  Stainless needs feedLight passes on 304 work-harden the surface and dull the tool.
• 3
  Superalloys cost timeTitanium and Inconel add cycle time, not just material cost.

Setup is where tolerance is won or lost. The part is located on three points, clamped without distorting it, and zeroed to a known feature. A vise on a thin plate will bow it. A soft jaw bored to the stock diameter will not.

For a second operation, do not re-zero from a raw edge. Cut a reference face or use a tooling ball so the second setup shares the first datum. On a 4-axis or 5-axis machine, the rotary table center becomes the datum, and the part is probed to find its actual position.

Thermal drift matters on long cycles. A machine that has been idle overnight will grow as the spindle warms. For tight work, run a warm-up cycle and check the first article before releasing the run.

• 1
  Locate then clampOver-clamping a thin wall bends it, then it springs back.
• 2
  Share the datumSecond ops should reference a machined feature, not raw stock.
• 3
  Warm up for tight workSpindle growth shows up on ±0.01 mm features.

A general tolerance block of ±0.1 mm covers most non-critical dimensions and keeps the price down. Reserve ±0.005 mm for bores, spigots, and mating faces. Every tight dimension adds inspection time, and inspection is a real cost line.

Surface finish follows the tool and the step-over. Ra 1.6–3.2 μm is normal as-machined. Ra 0.8–1.6 μm needs a finishing pass with a sharp tool and a small step-over. Ra 0.2–0.8 μm usually means a dedicated finish cut, a different insert, or a secondary operation.

Do not specify a fine finish on a surface that only needs to look good. A bead blast on an as-machined surface is cheaper than polishing and hides tool marks. Tell us the function, not just the number.

• 1
  General callout first±0.1 mm on most dimensions keeps cycle and inspection time low.
• 2
  Tight only where it matesBores and locating faces earn ±0.005 mm. Cosmetic faces do not.
• 3
  Finish has a cost curveRa 0.8 μm is a finish pass. Ra 0.2 μm is a separate operation.

The most expensive mistake is a missing thread callout. The machinist drills to the pilot diameter and the part arrives without usable threads. Write pitch and depth on every tapped hole.

The second is a deep, narrow pocket with sharp internal corners. The programmer has to use a small tool, the tool deflects, and the wall comes out tapered. Open the corner radius and the problem disappears.

The third is mixing models. An engineer edits the STEP file after sending the drawing, and the shop cuts to the drawing. Version-lock the files and note the revision on the drawing.

• 1
  Missing thread pitchM6 without 1.0 is an unfinished hole, not a thread.
• 2
  Sharp internal cornersSmall tools deflect. Radius the corner to fit the cutter.
• 3
  Two file versionsOne model, one drawing, one revision number.