2-Axis Milling: Contour and Pocket Toolpaths

2-Axis Milling: Contour and Pocket Toolpaths

What 2-Axis Toolpaths Do

In Mastercam, a 2-axis (2D) toolpath controls the cutter in the X and Y plane while depth steps are applied in the Z axis at fixed levels. No simultaneous 3-axis motion is needed. Two toolpaths dominate everyday 2D work: the contour toolpath, which follows an open or closed chain along a profile, and the pocket toolpath, which removes all material inside a closed boundary while respecting any islands inside that boundary.

Geometry Selection: Chaining

Before Mastercam can generate any toolpath, you must tell it which geometry to follow. This is called chaining. Click the chain icon and select connected line/arc entities in the order you want the tool to travel. Mastercam highlights the chain direction with an arrow. For a contour, direction controls which side of the line the tool cuts on. For a pocket, the outer boundary chains counterclockwise and islands chain clockwise by default, though Mastercam adjusts this automatically.

Verify the chain arrow before clicking OK. A reversed chain puts compensation on the wrong side and can gouge the part.

Cutter Compensation

Compensation shifts the tool centerline away from the programmed path so the cutter edge — not the center — follows the true part line. Mastercam offers two compensation types:

• Computer compensation (Wear OFF): Mastercam offsets the coordinates in the NCI/NC file. The machine runs the offset path directly, no controller offset register is used. Most common for CAM-generated programs.
• Control compensation (Wear ON): The posted G-code contains G41/G42 commands. The machine controller reads a tool radius offset register and applies the shift at runtime. This allows small adjustments for tool wear without regenerating the toolpath.

Compensation direction is either Left or Right relative to cutter travel direction. For a conventional outside contour machined climb-cut, compensation is typically set to Left. Always verify by checking the Backplot — the tool center line should be offset away from finished stock.

Entry and Exit Moves: Lead-In / Lead-Out

Plunging straight down to depth and immediately engaging the profile creates a witness mark and can chip an end mill. Use lead-in and lead-out arcs to ramp the tool tangentially onto and off the profile:

• A lead-in arc approaches the chain tangentially, so the cutter is already moving in the cut direction when it contacts the part surface.
• A lead-out arc exits tangentially, preventing a dwell mark at the endpoint.

A common starting value is an arc radius equal to 50–100% of the tool diameter. The arc must clear any islands or walls. In Mastercam, set radius, sweep angle (90° is typical), and linear length in the Lead In/Out tab.

Depth Cuts and Z Stepping

Removing full depth in one pass overloads the tool. Use depth cuts to step down in increments:

• Steel: maximum depth per pass ≤ 1× cutter diameter.
• Aluminum: maximum depth per pass ≤ 2× cutter diameter.

Enable depth cuts in the Depth Cuts tab, enter the Maximum Rough Step value, and Mastercam calculates the number of passes automatically. Enable Keep Tool Down if you want the cutter to stay in the pocket between Z steps rather than retracting.

Pocket Toolpath: Type and Cut Pattern

For a standard pocket with one or more bosses (islands), select Pocket type: Standard. Mastercam computes a series of offset passes that spiral or zigzag inward until the pocket is cleared.

Key parameters:

• Cut direction — Climb: The cutter engages material so chip thickness decreases through the cut. Climb milling produces a better surface finish and is preferred for carbide tooling on CNC machines. (Conventional cut is an alternative when backlash is a concern on older manual-style machines.)
• Stepover: The radial distance between successive passes. Set to 50% of tool diameter for roughing — this balances material removal rate and tool load.
• Finish pass: Enable one finishing pass with 0.010 in stock-to-leave to clean up the pocket walls after roughing. The finish pass uses the same tool; Mastercam adds a final pass at the full depth.

Stock-to-Leave and Finish Allowance

Stock-to-leave is the amount of extra material left on walls and/or floor after a roughing pass, to be removed by the finish pass. For the pocket finish pass, keep stock-to-leave at 0.015 in or less for typical precision work. Leaving too much requires excessive finish-pass cutting force; leaving too little removes the benefit of a separate finish pass.

Backplot and Verify

Before posting G-code, always Backplot the toolpath. Backplot animates the tool center movement so you can confirm:

• Compensation offset is on the correct side.
• Lead-in/lead-out arcs are present and tangent.
• Z depth steps are visible.
• No gouges (red highlights in Mastercam) exist.

If Backplot shows a gouge, do not post. Return to parameters, identify the conflict — often a lead-in arc too large for a tight corner — and correct it.

Safety in the CAM Lab

CAM lab work is programming, not live machining, but safety habits start at the computer:

• Never post and run unverified code. A gouge in Backplot becomes a crash on the machine.
• When you later run a program at the machine, follow lockout/tagout (LOTO) procedures for any tool change or setup adjustment with power off.
• Wear safety glasses any time you are on the shop floor near running machines, even if you are only observing.
• Keep chip hooks and brushes available; never use bare hands to clear chips from a running or recently stopped spindle.