How to Use a CNC Machine With Fusion 360

• 1
  What matters most
• 2
  Prepare the Model and Machine Before You Touch CAM
• 3
  Import the Model and Set Up the CAM Environment
• 4
  Generate Toolpaths for the CNC Machine With Fusion 360
• 5
  Where the Fusion 360 Workflow Usually Breaks Down
• 6
  Step-by-Step: From Toolpath to First Part
• 7
  Which Fusion 360 Toolpath Fits Your Part

Most failed jobs start before CAM. Open the model and look for features the tool cannot reach: internal corners sharper than the cutter radius, deep pockets narrower than 3× the tool diameter, and threads modelled with true helices when a simple tap callout would do. If a corner needs a 2 mm radius, do not model 0.5 mm and hope the machinist figures it out.

Collect machine data now, not later. You need the control type (Fanuc, Siemens, Haas, Mach3, LinuxCNC), the maximum spindle speed, the work envelope, and whether the machine has a fourth or fifth axis. A 4,000 mm gantry and a 500 × 500 × 450 mm vertical center take very different setups. Write the numbers down next to the CAM file.

Decide the material and stock form. Aluminium 6061-T6 cuts differently from 17-4PH stainless or Ti-6Al-4V. For aluminium you can run aggressive stepdowns; for titanium, keep radial engagement low and plan for more passes. If the part is a prototype, one block of stock is fine. If it is a production run, plan soft jaws or a fixture that repeats the zero point.

• 1
  Check tool accessAny pocket or corner must fit the smallest cutter you are willing to run.
• 2
  Note the controlThe post-processor is chosen by control, not by machine brand alone.
• 3
  Pick the stockLeave 0.5–1.0 mm on faces that will be finished later.
• 4
  Fix the zero pointDecide now whether X0 Y0 is a corner or the centre of a bore.

Fusion 360 accepts STEP, IGES, STL, and native F3D files. STEP is the safest choice for machined parts because it carries true surfaces and edges. STL is a mesh, so every curved face becomes triangles; if you must use STL, increase the mesh density before export or the toolpath will follow the facets.

After import, check the units. A part modelled in inches and imported into a millimetre document will be 25.4× too large. Fusion 360 usually asks, but not always. Measure one known dimension with the Inspect tool before you build any setup.

Create a Setup in the CAM workspace. Select the CNC machine from the library if yours is listed, otherwise choose Manual and fill in the travel limits. Set the Work Coordinate System to the point the operator will touch off. For a vice job, that is usually the top-left corner of the stock at Z0. For a second-op on a fixture, it may be a bore centre.

Define the stock. Use Relative size to add 1–2 mm on all sides, or Model size if the part is already the finished block. For castings or forgings, select From Solid and pick the as-received body. Wrong stock height is the most common cause of a first pass that cuts air or buries the tool.

• 1
  STEP over STLTrue surfaces give cleaner toolpaths on curved geometry.
• 2
  Verify unitsMeasure a known feature immediately after import.
• 3
  Set WCS to the touch-off pointMatch what the operator will actually indicate.
• 4
  Stock from solid for castingsDo not assume a rectangular block when the blank is not one.

Start with 2D operations for prismatic parts. Face the top, then use 2D Adaptive Clearing for the roughing pass. On aluminium 6061, a 10 mm three-flute carbide end mill can run 0.5–1.0 mm radial engagement and 5–10 mm axial depth at 8,000–12,000 rpm. On 304 stainless, drop the surface speed to roughly one third and keep the radial engagement at 5–8% of the tool diameter.

Use 3D Adaptive or 3D Pocket for curved surfaces that 2D cannot reach. These toolpaths follow the model shape and are slower to calculate but safer on complex geometry. For finishing, Scallop or Parallel gives a controlled stepover; on a 5-axis machine, Swarf and Multi-Axis Contour let the tool shank clear the part.

Drilling and tapping are separate operations. Select the hole faces, choose the cycle (drilling, peck, tap), and set the peck depth to no more than one tool diameter. For a tapped hole, use the Tap cycle and let the post output a rigid tapping block if the control supports it. Hand-tapping after machining is slower and less repeatable.

Set the feeds and speeds per tool, then check the engagement numbers in the toolpath summary. If the load is above what the machine or tool can take, reduce the stepover before you reduce the feed. RPM and feed can be tuned on the machine; a broken tool cannot.

• 1
  Rough with adaptiveConstant engagement keeps tool load predictable.
• 2
  Finish with scallop or parallelStepover controls the surface finish directly.
• 3
  Peck no deeper than 1×DChip evacuation matters more than cycle time on deep holes.
• 4
  Check load before postingThe summary shows whether the cut is within the tool's range.

The first failure point is the post-processor. A generic Fanuc post may output a G28 that your Haas control interprets differently, or a tool change that does not match the carousel. Test the post on a simple facing program before you trust it on a complex part. Keep a known-good post for each control in the shop.

The second is the WCS versus the physical setup. If CAM assumes Z0 is the top of the stock and the operator touches off on the vice jaw, every Z move is offset by the stock height. Write the WCS assumption on the setup sheet and make the operator verify it before cycle start.

The third is tool deflection on deep cuts. Fusion 360 calculates the toolpath from the model, but it does not know your holder runout or the actual rigidity of the setup. On a 4×D reach with a 6 mm tool, expect to reduce the stepover and add a spring pass. The CAM numbers are a starting point, not a guarantee.

The fourth is stock variation. If you are machining a casting, the as-received surface may be 1–2 mm off the nominal. Use the From Solid stock option and add a check pass before the finishing toolpath. A single setup that assumes a perfect block will cut air on one side and overload on the other.

• 1
  Test the post firstRun a simple program before the complex one.
• 2
  Write the WCS on the setup sheetThe operator cannot guess what CAM assumed.
• 3
  Expect deflection on long toolsReduce stepover and add a spring pass.
• 4
  Check the blank, not the modelCastings and forgings vary from nominal.