Causes and Solutions for Overcutting in CNC Machining

In CNC machining, overcutting due to tool vibration often occurs at corner areas of the parts, leading to product appearance defects and tolerance issues. By carefully selecting tools and optimizing machining methods, the risk of overcutting can be effectively reduced. This article analyzes common factors that cause tool vibration and overcutting and provides effective solutions.

How End Mill Helix Angle Impacts Overcutting?

The helix angle of an end mill plays an important role in managing tool vibration and preventing overcutting during machining. Because it greatly influences machining performance.

The influence of the helix angle on the machining effect can be analyzed from several aspects, including the characteristics of the material being cut, cutting resistance, machining accuracy, and tool life.

Material Characteristics

Low-hardness materials: Large-helix-angle tools (e.g., 45° three-flute end mills) are preferred due to their sharper edges and larger rake angles.
High-hardness materials: Small-helix-angle tools are ideal as they offer stronger edge rigidity due to smaller rake angles.

Cutting Resistance

The tangential resistance decreases as the helix angle of the end mill increases, while the axial resistance increases with the enlargement of the helix angle.

Machining Precision

The larger the helix angle of the end mill, the better the accuracy of perpendicularity, flatness, and roughness of the machined surface, but the chip evacuation performance is poorer. For grooves with a cutting width close to the tool diameter, small-helix-angle tools are recommended.

Tool Life

With a larger helix angle, the contact line between the workpiece and the cutting edge increases, reducing load per unit area. However, higher axial cutting forces may loosen the tool and cause overcutting. Stable tool holders should be used in such cases.

Small and Large Helix Angle End Mill:

• Small-helix-angle end mills: Short cutting edges. (blue line)

• Large-helix-angle end mills: Long cutting edges. (red line)

Principles of Tool Usage to Prevent Overcutting

Proper tool usage is another factor affecting the occurrence of overcutting due to tool vibration. Follow these principles and monitor machining conditions:

• Controlling Tool Runout: Measure the tool runout accurately, and the smaller the tool swing is the better. This helps to improve machining accuracy, surface finish, and tool life.
• Optimizing Tool Extension Length: It is better that the shorter the length of the tool extends beyond the chuck. If a longer tool extension is required, the speed, feed rate, or cutting depth should be reduced.

• Address Unusual Vibrations: Lower the feed rate if unusual vibrations or noise occur until conditions stabilize.
• Avoid Emergency Stops or Power Failures: As shown in the picture below, Figure A is the state of the tool when machining a relatively flat place. When machining reaches Point B and a sudden stop is made, preparing for reverse machining, the tool will undergo deformation due to inertia. This can result in the occurrence of overcutting due to tool vibration at Point B.

Manage Tool Deformation to Minimize Overcutting

Tool deformation can also lead to tool vibration and overcutting.

• σ = Tool deformation amount
• L = Tool mounting length
• D = Tool diameter
• P = Force acting on the tool

From the above formula, we can identify three main factors that influence tool deformation:

• Tool Mounting Length (L): The deformation amount of the tool has a cubic relationship with the tool mounting length. Therefore, the tool mounting length should be shortened as much as possible.
• Tool Diameter (D): The deformation amount of the cutting tool is inversely proportional to the diameter. To reduce deformation, consider using tools with a larger diameter when possible, as this will significantly decrease the deformation amount.
• Force Acting on the Tool (P): The deformation amount of the tool is directly proportional to the force acting on it during processing. Reducing the force acting on the tool can decrease the chance of chatter. Therefore, reducing the contact area between the tool and the workpiece to lower the force can prevent the occurrence of overcutting due to tool vibration.

Programming Strategies to Avoid Tool Vibration and Overcutting

Programming strategies also impact tool vibration. Especially for deep cavities and complex geometries, consider the following:

Select Appropriate Cutting Tools

Choose suitable cutting tools based on the product structure, preferably using larger tools for roughing. Avoid using excessively long small tools for rough cutting, as this can easily cause micro-vibrations in the tool, leading to overcutting.

Reserve Uniform Allowance

After rough cutting, a program of chamfering the corners should be added to ensure that the allowance is uniform. For corners with a large allowance, rounding them off and increasing the R-angle can reduce the load on the cutting tool at the corner. It helps lower the overcutting due to tool vibration.

Optimized Cutting Method

During roughing, the cutting method should alternate between climb milling and conventional milling. When the side cutting edge engages with many materials during rough cutting in deep cavities, conventional milling can cause chatter and slight tool runout. If the allowance reserved for roughing is insufficient, this can easily lead to overcutting. Therefore, the most appropriate method to choose is climb milling.

Avoid Missed Cutting

For geometric parts with special surface intersections, it is easy to issues such as the tool path cutting into the geometric interior. This means “missed cutting,” where the tool penetrates into the geometric parts, leading to overcutting. The optimized method is adjusting tool path or tolerances.

Correct Entry and Exit Toolpaths

When following a 2D tool path, using arcuate tool entry and exit requires avoiding the workpiece to ensure reasonable entry and exit positions. When following a 3D tool path, if the arcuate tool entry and exit are defined, the system will automatically avoid the workpiece during tool exit. But this may result in a distorted toolpath. However, using a G0 code(rapid positioning) move for tool exit may result in slight overcutting.

Tool Compensation Direction

When using Mastercam to follow a 2D tool path for profiling, we typically apply left compensation for climb milling. Otherwise, incorrect compensation will cause collisions or overcuts.

Tool Geometry

When milling with a ball-end mill, if the milling depth is less than the tool’s chamfer radius, it is prone to overcutting at the start. The solution is to ensure that the milling depth is greater than the tool’s chamfer radius. Or alternatively, not to use a ball-end mill for specific applications.

Conclusion

The issue of tool vibration and overcutting in CNC machining can be comprehensively addressed by optimizing tool selection, adhering to tool usage principles, and paying attention to programming details. This not only effectively reduces the probability of overcutting due to tool vibration, but also enhances processing accuracy, shortens processing time, and improves surface roughness.