What Is CNC Contour Milling? Feed-Path and Cutting-Parameter Design

In CNC machining, the path followed by the cutter location point relative to the part is called the machining path. Path design directly affects dimensional accuracy and surface roughness. A suitable path should follow four principles:

1. It should achieve the required accuracy and surface finish while maintaining high efficiency.
2. It should simplify numerical calculations and reduce programming work.
3. It should be as short as practical to reduce both program blocks and non-cutting time.
4. It should reflect the available stock allowance and the rigidity of the machine, tool, and workpiece.

Lead-In, Lead-Out, and Cutter Compensation

Contour milling generally requires cutter-radius compensation. The toolpath should establish compensation before the cutter enters the workpiece and cancel it only after the cutter has left the workpiece.

When entering or leaving a profile, the cutter should follow a line or arc tangent to the contour. Tangential entry and exit avoid the tool marks that can result from a direct normal approach and help keep the finished contour smooth.

One simple method establishes radius compensation while the cutter moves in a straight line from point S toward the contour. The cutter later returns to S in a straight line, and compensation is canceled during the return. This direct approach is efficient, but contact at the point where the cutter meets the profile can leave a visible witness mark. It is therefore more suitable when contour requirements are not stringent.

For a high-quality contour, radius compensation is established during a straight move from point S that does not touch the finished profile. With compensation active, an arc then brings the cutter naturally and tangentially into the circular contour. After the contour is complete, the exit sequence is reversed, and compensation is canceled during the final straight return move.

When finish milling an external contour, the cutter should enter tangentially from outside the profile and withdraw along a tangent after machining is complete.

Cutting Parameters for Contour Milling

Axial and Radial Depth of Cut

Flute length, or side-cutting-edge length, determines the maximum cutting depth. In practice, the axial depth of cut in the Z direction (a_p) should not exceed 1.5 times the cutter diameter. The radial depth of cut (a_w) should not exceed the cutter radius.

A smaller-diameter end mill requires a shallower cutting depth to maintain adequate rigidity.

When an end mill roughs an unmachined surface, a serrated roughing end mill may be used for heavy cutting if the machine-tool-workpiece system permits it. If a large stock allowance must be removed, a larger-diameter, shorter end mill is preferable.

This combination helps prevent cutter chatter and deflection during heavy cutting, or at least keeps both effects to a minimum.

Feed Rate

Different operating conditions require different feed rates. Feed motion can be divided into two types:

• Rapid-traverse rate: the feed rate used for non-cutting travel.
• Machining feed rate: the working feed used during entry, exit, and cutting.

To improve efficiency and reduce non-cutting time, rapid traverse should be as fast as practical and normally uses the maximum rate allowed by the machine.

The machining feed rate (v_f) is related to cutter speed (n), number of teeth (z), and feed per tooth (f_z) as follows:

v_f = f_z · z · n      Equation (5-1)

where:

• v_f is the feed rate;
• f_z is the feed per tooth, in millimeters per tooth (mm/tooth);
• z is the number of cutter teeth; and
• n is the cutter rotational speed.

Feed per tooth (f_z) is selected mainly according to the mechanical properties of the workpiece material, cutter material, and required surface roughness.

As workpiece strength and hardness increase, f_z should decrease; as they decrease, f_z can increase. A carbide cutter normally permits a higher feed per tooth than a comparable high-speed steel cutter.

A finer surface-roughness requirement calls for a smaller f_z. A low-rigidity workpiece or a cutter with limited strength also requires a smaller value.

Feed Rate on Circular Arcs

During circular interpolation, the actual feed rate at the cutting point (v_T) differs from the selected feed rate at the cutter center (v_f) because of the arc radius.

For an external arc, the actual feed rate at the cutting point is:

v_T = RR + r · v_f

Therefore: v_T < v_f

For an internal arc, the actual feed rate at the cutting point is:

v_T = RR − r · v_f

Therefore: v_T > v_f

If R ≈ r, the actual feed rate at the cutting point becomes extremely high and may damage the tool or workpiece. The influence of arc radius must therefore be considered when the programmed feed rate is selected.

Other special factors also affect feed-rate selection. In contour machining, for example, inertia or deformation in the machining system can produce overtravel or undertravel at a corner.

If the cutter moves from point A toward point B at a high feed rate, inertia may cause overtravel and overcut at corner B. Excess material is removed from the corner, creating a contour error.

A variable feed rate can address this problem. Reduce the feed appropriately before reaching the corner, then increase it gradually after the cutter has passed the corner.

End-Mill Spindle Speed

When machining steel, an indexable carbide end mill should generally run at a higher spindle speed than a standard HSS cutter.

As spindle speed increases during carbide machining, the temperature of the steel in contact with the cutting edge also increases. The material softens locally, creating more favorable cutting conditions.

The spindle speed used with a carbide cutter is commonly three to five times that used with a standard HSS cutter. Running an indexable carbide end mill at too low a spindle speed can cause the carbide to chip or even fail.

For a high-speed steel cutter, however, an excessively high spindle speed accelerates tool wear.

Milling speed can also be selected by referring to an appropriate cutting-speed table.

[IMAGE PLACEHOLDER: Reference table for milling cutting speeds]

Figure: Reference table for milling cutting speeds

Chatter and Cutting-Parameter Correction

An end mill may chatter during machining. Common causes include insecure tool clamping, excessive cutter overhang from the holder, excessive depth of cut or feed rate when machining thin walls, and cutter deflection.

Vibration causes uneven engagement around the end mill’s peripheral cutting edges. The actual cutting load can exceed the intended value, reducing machining accuracy and tool life.

When vibration occurs, reduce both cutting speed and feed rate. If significant vibration remains after both have been reduced by 40%, reduce the depth of cut.

If chatter still persists, inspect the machining method and the rigidity of the setup.