How to Make CNC Machine Program

• 1
  Key takeaways
• 2
  Define part requirements and DFM constraints
• 3
  Choose manual programming or CAM software
• 4
  Prepare the CAD model for machining
• 5
  Generate toolpaths and set cutting parameters
• 6
  Simulate, post-process, and prove out the code
• 7
  Seven steps from model to proven G-code
• 8
  Manual programming vs CAM by part type

Every program starts as a set of decisions, not as a line of code. Before opening CAM, list the functional surfaces, the datum scheme, and the tolerances that actually matter. A bearing bore at ±0.005 mm and a clearance hole at ±0.2 mm should never get the same finishing strategy. Write the critical dimensions down and mark them on the drawing.

Then check the part for features that fight the cutting tool. Deep pockets narrower than 4× the tool diameter, sharp internal corners, and threads that stop against a shoulder all drive cost. Adding a fillet slightly larger than the tool corner radius lets you use a bigger, stiffer cutter. It is a five-minute model change and often removes a second operation.

Material sets the cutting parameters. Aluminum 6061 and 7075 run fast with high rake angles; 316L stainless work-hardens if you dwell, so keep the feed per tooth up and never let the tool rub. Titanium Ti-6Al-4V and Inconel need lower surface speed and more coolant pressure. Choose the insert grade and coating after the material, not before.

• 1
  Datum strategyPick datums that exist on the raw stock so the first setup can be probed.
• 2
  Tolerance mapSeparate critical dimensions from cosmetic ones on the setup sheet.
• 3
  Wall thicknessBelow 0.8 mm in aluminum, plan a finishing pass with light radial engagement.
• 4
  Thread depthKeep at least 2× pitch of full thread for reliable gauging.

Manual G-code is still the right answer for simple 2.5D work: face milling, drilling patterns, a single counterbore, or a quick fixture plate. You can write it at the machine, edit it in seconds, and there is no post-processor to debug. For a part with six holes and two pockets, CAM setup time often exceeds the time saved.

CAM takes over as soon as you have 3D surfaces, blended fillets, or more than one setup. Modern CAM handles rest material, tool holder collision, and adaptive clearing that keeps radial engagement constant. On a 5-axis part with undercuts, hand-writing code is not realistic. The trade is setup time versus cutting time: complex parts usually justify the CAM session.

A middle path works well for shops that run the same families repeatedly. Build a template with stock setup, WCS, tool library, and feeds already loaded. The programmer then only picks geometry and adjusts the stepover. Templates cut programming time and, more importantly, stop parameters from drifting between operators.

• 1
  Manual is fine forFacing, spot drilling, bolt circles, simple slots, fixture plates.
• 2
  CAM is required for3D contoured surfaces, rest machining, 5-axis simultaneous, complex fixturing.
• 3
  Hybrid approachCAM for the geometry, hand edits for entry points and retract moves.

Import the model, then delete what the machine does not need. Suppressed features, cosmetic logos, and internal threads modeled at nominal size all create noise. If the part is a weldment or an assembly, collapse it to a single solid. Any gap or sliver face will produce a broken toolpath that looks fine in preview and fails at the machine.

Define the stock next. A 100 × 100 × 20 mm aluminum block for a small enclosure leaves enough material for clamping and for a 1-2 mm facing cut on each side. Add stock deliberately: 2 mm on machined faces, 5 mm on saw-cut faces, and more where the part will be held in a vise. Undersized stock is the most common reason a program has to be rewritten.

Set the work coordinate system at a feature you can touch off or probe. A corner of the stock, the center of a bored hole, or a dedicated fixture boss all work. Avoid using a theoretical intersection that only exists in the model. If the operator cannot find the WCS with an edge finder or a probe, the program will run offset.

• 1
  Heal the geometryRun a model check for gaps, overlapping faces, and zero-thickness walls.
• 2
  Stock plus2 mm on finished faces, 5 mm on saw cuts, more where clamping is needed.
• 3
  WCS placementUse a probeable corner or bore, never a theoretical point.

Roughing first. Adaptive or trochoidal clearing holds radial engagement around 10-15% of tool diameter and axial depth up to 2-3× diameter in aluminum. That combination removes material fast without burying the cutter. On stainless and titanium, drop axial depth to 1× diameter and keep the feed per tooth at 0.05-0.1 mm so the edge cuts instead of rubs.

Finishing decides surface finish. A stepover of 5-10% of tool diameter gives a scallop height in the Ra 0.8-1.6 μm range on most aluminum parts. Push stepover to 20% and you will see witness lines under light. If the drawing calls for Ra 0.2-0.8 μm, plan a separate finish pass with a smaller stepover or a different tool, and expect the cycle time to rise.

Order the operations so the part stays rigid. Rough both sides, then finish the faces that locate the second setup, then finish everything else. Drill before you ream, ream before you bore. Cut the outside profile last when the part is thin, and leave tabs or a sacrificial web so the part does not move when the contour releases it.

• 1
  Roughing stepover10-15% of tool diameter with adaptive clearing, 60-70% for conventional.
• 2
  Finishing stepover5-10% of tool diameter for Ra 0.8-1.6 μm; less for finer finishes.
• 3
  Operation orderRough, locate, finish critical faces, then profile and release.
• 4
  Thin wallsLeave tabs or a web; a released 0.8 mm wall will spring.

Simulation must include the holder, the chuck or vise, and the fixture. Most crashes are not the tool hitting the part, they are the holder hitting a clamp during a rapid move. Check every rapid at full speed in the simulation, then check the retract plane between operations. A clearance plane 5 mm above the stock is safer than 1 mm and costs almost nothing.

Post-processing converts the internal toolpath into machine-specific G-code. The post must know the control model, the axis configuration, and whether the machine uses G54 or a pallet offset. A generic post will produce code that runs but may reverse an axis or output the wrong arc format. Test a new post on a scrap block before it touches a production part.

Prove out in three stages. First, run the program with the tool offset 5-10 mm above the stock and watch the position display. Second, cut the first part with feed override at 50% and single block on. Third, measure the critical dimensions and adjust cutter compensation or wear offsets from the inspection report, not from feel. Record the offset change so the next run starts from a known state.

• 1
  Simulate fixturesHolder and clamp collisions are the most common crash cause.
• 2
  Clearance plane5 mm above stock for rapids; more if the fixture is tall.
• 3
  Post validationCut a scrap block first when a post or machine is new.
• 4
  Offset disciplineAdjust wear offsets from measured data and log the change.