Precision Bevel Machining Methods with UG CAM Systems

This paper presents two primary solutions for optimizing the efficiency and quality of chamfering in UG CAM. The first solution involves directly forming the chamfer profile using a standard forming tool, while the second utilizes a contoured tool with a radius profile to create the chamfer.

The document provides detailed methods for creating these chamfers, highlights key application points, and outlines strategies for setting tool tracking points for both standard and custom chamfering tools. Additionally, it offers a systematic summary of the characteristics associated with various chamfering methods, including plane chamfering, contour chamfering, and hole chamfering.

The aim of this paper is to serve as a comprehensive technical reference for process engineers, assisting them in enhancing both the efficiency and quality of chamfering processes.

 

01 Introduction

Chamfering is commonly used in the manufacturing of mechanical products. It serves multiple purposes: it removes burrs from machined parts, enhances product aesthetics, facilitates assembly, and reduces stress concentration effectively. There are various types of chamfers, including oblique chamfers, such as 60°, 90°, and 120° angles (often used for hole openings), round chamfers (typically found on the tops of end face grooves), and special-shaped chamfers that consist of a combination of straight and curved lines.

As the machinery manufacturing industry seeks higher precision and quality in products, process engineers must be proficient in various chamfering methods under different operating conditions. They should continuously research and optimize machining processes to meet these demands.

UG NX software offers significant advantages for generating chamfering programs, providing an efficient solution for chamfering various parts. Currently, chamfering mainly involves two machining modes: forming the chamfer profile directly with a dedicated forming tool or contouring the chamfer profile using an R-shaped tool. Therefore, it is crucial to conduct in-depth research into the characteristics of chamfering tools and the machining methods that utilize different tools to enhance chamfering quality and efficiency.

 

02 Chamfering Tools

2.1 Forming Chamfering Tools
Chamfering tools are a specific type of forming tool used to create chamfers. There are various methods to manufacture a chamfering tool, but we have found that utilizing the “chamfer mill” function in the “mill planar milling” operation, along with the “counter sink” function in the “hole making” operation of UG software, is both simple and intuitive. This approach effectively meets production needs and satisfies all requirements for creating chamfering tools. Figure 1 illustrates the process of creating a forming chamfering tool.

 

In practical applications, it is important to understand the distinction between the actual tool and the theoretical tool, especially when the tool tip is sharp. The actual tool tip is rounded, which means that the highest point of the tool during the tool-setting process does not correspond to the theoretical tool tip. This discrepancy can lead to issues during machining.

As illustrated in Figure 2, the difference between the theoretical and actual tools can result in excessive chamfers if programming is based solely on the theoretical tool tip. To prevent this, it is advisable to calculate the actual tool tip using trigonometric functions before beginning machining. Alternatively, one can use the theoretical tool tip for programming while using the actual tool tip for setting the tool. This approach ensures greater machining accuracy.

 

2.2 Custom Chamfer Tools

Both chamfer and contoured corner tools are custom tools that can be created in the “MILL_USER_DEFINED” section (Custom Tools) under the “mill_planar” operation. A custom tool is formed by rotating a generatrix around a centerline. The generatrix typically consists of a combination of straight and circular segments.

Straight segments are represented in polar coordinates, defined by the line length (LL) and the line/arc start angle (LA). Circular segments are described by the arc radius (AR) and arc sweep (AS). For complex curved segments, continuous small line or arc segments can be used to approximate the shape. As long as the tool’s generatrix can be mathematically defined, it can be quantified using four parameters: line length, angle, radius, and sweep.

It is important to note that custom chamfer tools are suitable only for 2D planar contour milling. A visual example of a custom tool is shown in Figure 3.

 

2.3 Tool Tracking Points

Regardless of the method used to generate tools, tracking points can be established in the tool dialog box. Tool tracking points act as reference points, precisely controlling the contact point between the tool and the chosen workpiece. You can set multiple tracking points for a single tool. Properly configuring and selecting these tracking points simplifies programming operations. It is important to note that tool tracking points are independent of the final program output. The process for setting tracking points is illustrated in Figure 4.

 

03 Form Tool Machining

3.1 Drilling

When drilling, clearly specify the top surface and hole in the drilling interface. In the “Standard Drill” cycle, edit the parameters and set the shoulder depth to 0. When setting the tool, adjust the tool length to the location on the tool’s tapered face where the maximum chamfer diameter aligns with the part. If the same chamfering tool is used to create multiple chamfers of varying depths, set the tool shoulder location to the tool length during the tool setting process. In the “Standard Drill” cycle, define the shoulder depth value (typically a negative value) according to the chamfer depth. This method is appropriate when the maximum chamfering tool diameter is equal to or larger than the maximum chamfer diameter of the hole. It provides advantages such as fewer toolpaths, simpler programming, and improved machining efficiency.

 

3.2 Plane Milling and Plane Contour Milling

When performing plane prototype CNC milling, select the chamfered edge on the end face in the “Specify Part Boundary” interface and adjust the “Tool Side” setting accordingly. In the “Specify Bottom Face” setting, choose the chamfered edge on the wall of the hole and apply a small offset toward the depth of the hole to minimize tool setting errors.

For plane contour milling, select the end face in the “Specify Part Boundary” section. Again, select the chamfered edge on the wall of the hole and apply an offset in the “Specify Bottom Face” section.

Plane milling is mainly used for chamfering open boundaries, while plane contour milling is more suitable for chamfering closed boundaries. Figure 5 illustrates the applications of plane milling and plane contour milling.

 

3.3 Hole Backcut Milling

In the “Holl_Making” interface, begin by selecting a backcut milling cutter. Next, choose the chamfer feature under “Specify Feature Geometry.” In the “Drive Point” section, select the tool tracking point and set the starting position as the depth offset in the chamfer reference. It is important to ensure that the tool tracking point aligns with the depth offset positions for both the minimum and maximum diameters specified in the chamfer reference. By effectively managing these three relationships, you can simplify the programming process and enhance efficiency. The hole chamfer is illustrated in Figure 6.

 

3.4 Reverse Chamfering

In the Contour Milling interface, choose the intersection of the chamfer and the top surface of the inner groove under “Specify Part Boundary.” Select a custom tool and designate the edge point shown in Figure 4 as the driving point to perform reverse chamfering. The reverse chamfering process using Contour Milling is illustrated in Figure 7.

 

04 Machining with R-Type Tools

R-type tools include ball-end cutters, straight-tooth end mills with R-type geometry, and T-type milling cutters designed with R-type features.

4.1 Deep Contour Milling

In the “Deep Contour Milling” interface, start by selecting the chamfered surface under “Specify Cutting Area.” For the “Common Cut Depth Per Cut,” choose “Constant” and enter a value of 0.05 for “Maximum Distance.” Next, select either a ball-end cutter or a straight-tooth end mill featuring R-type tools.

In the Connections tab of the Cutting Parameters dialog box, select “Inclined Feed Along the Part” for the “Layer to Layer” option and set the “Ramp Angle” to 1 to achieve contoured chamfering. An example of Deep Contour Milling with contoured chamfering is illustrated in Figure 8.

 

4.2 Fixed Axis Contour Milling

In the “Fixed Contour Milling” interface, begin by selecting either a ball-end mill or a straight-tooth end mill with an R specification. When using the “Surface Area” drive method, choose the chamfered surface in the “Specify Drive Geometry” section and set the “Surface %” for the Cutting Area. Access the Surface Percentage Method dialog box and configure the Start Step Size to -10 and the End Step Size to 110. This configuration will extend the tool path beyond the chamfered surface. The machined surface area is illustrated in Figure 9.

For the “Streamline” drive method, select “Part” as the Component, choose the chamfered surface as the Cutting Area, specify the Cutting Direction, and select either Spiral or Planar Spiral as the Cutting Mode. Set the Cutting Method to Constant Step Size and enter 0.1 for the Maximum Distance. Additionally, under the Trim and Extend section, adjust the Start Step Size to -5 and the End Step Size to 105. This will also extend the tool path beyond the chamfered surface. The streamlined process is depicted in Figure 10.

 

4.3 Back Chamfering

Both the Curved Area and Streamline methods under “Fixed Contour Milling” can be used for back chamfering. The basic settings are the same as those described in section 4.2. Use a T-type milling cutter with an R designation. Select the projected vector as the distance line, the specified vector as the centerline of the hole, and the specified point as the center of the hole. The back chamfering milling process is illustrated in Figure 11.

 

05 Conclusion

This paper systematically examines two machining methods: one involves using UG CAM to directly create the chamfer contour with a forming tool, while the other utilizes an R-shaped tool to achieve the same contour. Additionally, the paper consolidates practical machining experiences. UG CAM is both powerful and versatile, offering a diverse range of chamfering techniques. We hope this will serve as a useful reference for colleagues in the field and help advance the development of chamfering technology in machining.

 

 

 

If you want to know more or inquiry, please feel free to contact info@anebon.com

Anebon’s goal is to understand the excellent craftsmanship in manufacturing and to provide top-notch support to domestic and international clients wholeheartedly for 2024 in high-quality stainless steel, aluminum, and high-precision metal stamping products, CNC machining, and die casting zinc alloy for aerospace.