Effective Application of Forming Angle Milling Cutters in Machining
Angle milling cutters are frequently employed in the machining of small inclined surfaces and precision components across various industries. They are particularly effective for tasks such as chamfering and deburring workpieces.
The application of forming angle milling cutters can be explained through trigonometric principles. Below, we present several examples of programming for common CNC systems.
1. Preface
In actual manufacturing, it is often necessary to chamfer the edges and corners of products. This can typically be accomplished using three processing techniques: end mill layer programming, ball cutter surface programming, or angle milling cutter contour programming. With end mill layer programming, the tool tip tends to wear out quickly, leading to a reduced tool lifespan [1]. On the other hand, ball cutter surface programming is less efficient, and both end mill and ball cutter methods require manual macro programming, which demands a certain level of skill from the operator.
In contrast, angle milling cutter contour programming only requires adjustments to the tool length compensation and radius compensation values within the contour finishing program. This makes angle milling cutter contour programming the most efficient method among the three. However, operators often rely on trial cutting to calibrate the tool. They determine the tool length using the Z-direction workpiece trial cutting method after assuming the tool diameter. This approach is only applicable to a single product, necessitating recalibration when switching to a different product. Thus, there is a clear need for improvements in both the tool calibration process and programming methods.
2. Introduction of commonly used forming angle milling cutters
Figure 1 shows an integrated carbide chamfering tool, which is commonly used to deburr and chamfer the contour edges of parts. Common specifications are 60°, 90° and 120°.
Figure 1: One-piece carbide chamfering cutter
Figure 2 shows an integrated angle end mill, which is often used to process small conical surfaces with fixed angles in the mating parts of parts. The commonly used tool tip angle is less than 30°.
Figure 3 shows a large-diameter angle milling cutter with indexable inserts, which is often used to process larger inclined surfaces of parts. The tool tip angle is 15° to 75° and can be customized.
3. Determine the tool setting method
The three types of tools mentioned above utilize the bottom surface of the tool as the reference point for setting. The Z-axis is established as the zero point on the machine tool. Figure 4 illustrates the preset tool setting point in the Z direction.
This tool setting approach helps maintain consistent tool length within the machine, minimizing the variability and potential human errors associated with trial cutting of the workpiece.
4. Principle Analysis
Cutting involves the removal of surplus material from a workpiece to create chips, resulting in a workpiece with a defined geometric shape, size, and surface finish. The initial step in the machining process is to ensure that the tool interacts with the workpiece in the intended manner, as illustrated in Figure 5.
Figure 5 Chamfering cutter in contact with the workpiece
Figure 5 illustrates that to enable the tool to make contact with the workpiece, a specific position must be assigned to the tool tip. This position is represented by both horizontal and vertical coordinates on the plane, as well as the tool diameter and the Z-axis coordinate at the point of contact.
The dimensional breakdown of the chamfering tool in contact with the part is depicted in Figure 6. Point A indicates the required position. The length of line BC is designated as LBC, while the length of line AB is referred to as LAB. Here, LAB represents the Z-axis coordinate of the tool, and LBC denotes the radius of the tool at the contact point.
In practical machining, the tool’s contact radius or its Z coordinate can be preset initially. Given that the tool tip angle is fixed, knowing one of the preset values allows for the calculation of the other using trigonometric principles [3]. The formulas are as follows: LBC = LAB * tan(tool tip angle/2) and LAB = LBC / tan(tool tip angle/2).
For instance, using a one-piece carbide chamfering cutter, if we assume the tool’s Z coordinate is -2, we can determine the contact radii for three different tools: the contact radius for a 60° chamfering cutter is 2 * tan(30°) = 1.155 mm, for a 90° chamfering cutter it is 2 * tan(45°) = 2 mm, and for a 120° chamfering cutter it is 2 * tan(60°) = 3.464 mm.
Conversely, if we assume the tool contact radius is 4.5 mm, we can calculate the Z coordinates for the three tools: the Z coordinate for the 60° chamfer milling cutter is 4.5 / tan(30°) = 7.794, for the 90° chamfer milling cutter it is 4.5 / tan(45°) = 4.5, and for the 120° chamfer milling cutter it is 4.5 / tan(60°) = 2.598.
Figure 7 illustrates the dimensional breakdown of the one-piece angle end mill in contact with the part. Unlike the one-piece carbide chamfer cutter, the one-piece angle end mill features a smaller diameter at the tip, and the tool contact radius should be calculated as (LBC + tool minor diameter / 2). The specific calculation method is detailed below.
The formula to calculate the tool contact radius involves using the length (L), angle (A), breadth (B), and the tangent of half the tool tip angle, summed with half the minor diameter. Conversely, obtaining the Z-axis coordinate entails subtracting half of the minor diameter from the tool contact radius and dividing the result by the tangent of half the tool tip angle. For instance, using an integrated angle end mill with specific dimensions, such as a Z-axis coordinate of -2 and a minor diameter of 2mm, will yield distinct contact radii for chamfer milling cutters at various angles: a 20° cutter yields a radius of 1.352mm, a 15° cutter offers 1.263mm, and a 10° cutter provides 1.175mm.
If we consider a scenario where the tool contact radius is set at 2.5mm, the corresponding Z-axis coordinates for chamfer milling cutters of different degrees can be extrapolated as follows: for the 20° cutter, it calculates to 8.506, for the 15° cutter to 11.394, and for the 10° cutter, an extensive 17.145.
This methodology is consistently applicable across various figures or examples, underscoring the initial step of ascertaining the tool’s actual diameter. When determining the CNC machining strategy, the decision between prioritizing the preset tool radius or the Z-axis adjustment is influenced by the aluminum component‘s design. In scenarios where the component exhibits a stepped feature, avoiding interference with the workpiece by adjusting the Z coordinate becomes imperative. Conversely, for parts devoid of stepped features, opting for a larger tool contact radius is advantageous, promoting superior surface finishes or enhanced machining efficiency.
Decisions regarding the adjustment of the tool radius versus augmenting the Z feed rate are based on specific requirements for the chamfer and bevel distances indicated on the part’s blueprint.
5. Programming Examples
From the analysis of the tool contact point calculation principles, it is evident that when utilizing a forming angle milling cutter for machining inclined surfaces, it is sufficient to establish the tool tip angle, the minor radius of the tool, and either the Z-axis tool setting value or the preset tool radius.
The following section outlines the variable assignments for the FANUC #1, #2, Siemens CNC system R1, R2, Okuma CNC system VC1, VC2, and the Heidenhain system Q1, Q2, Q3. It demonstrates how to program specific components using the programmable parameter input method of each CNC system. The input formats for the programmable parameters of the FANUC, Siemens, Okuma, and Heidenhain CNC systems are detailed in Tables 1 to 4.
Note: P denotes the tool compensation number, while R indicates the tool compensation value in absolute command mode (G90).
This article employs two programming methods: sequence number 2 and sequence number 3. The Z-axis coordinate utilizes the tool length wear compensation approach, whereas the tool contact radius applies the tool radius geometry compensation method.
Note: In the instruction format, “2” signifies the tool number, while “1” denotes the tool edge number.
This article employs two programming methods, specifically serial number 2 and serial number 3, with the Z-axis coordinate and tool contact radius compensation methods remaining consistent with those previously mentioned.
The Heidenhain CNC system allows for direct adjustments to the tool length and radius after the tool has been selected. DL1 represents the tool length increased by 1mm, while DL-1 indicates the tool length decreased by 1mm. The principle for using DR is consistent with the aforementioned methods.
For demonstration purposes, all CNC systems will utilize a φ40mm circle as an example for contour programming. The programming example is provided below.
5.1 Fanuc CNC system programming example
When #1 is set to the preset value in the Z direction, #2 = #1*tan (tool tip angle/2) + (minor radius), and the program is as follows.
G10L11P (length tool compensation number) R-#1
G10L12P (radius tool compensation number) R#2
G0X25Y10G43H (length tool compensation number) Z0G01
G41D (radius tool compensation number) X20F1000
Y0
G02X20Y0 I-20
G01Y-10
G0Z50
When #1 is set to the contact radius, #2 = [contact radius - minor radius]/tan (tool tip angle/2), and the program is as follows.
G10L11P (length tool compensation number) R-#2
G10L12P (radius tool compensation number) R#1
G0X25Y10G43H (length tool compensation number) Z0
G01G41D (radius tool compensation number) X20F1000
Y0
G02X20Y0I-20
G01Y-10
G0Z50
In the program, when the length of the part’s inclined surface is marked in the Z direction, R in the G10L11 program segment is “-#1-inclined surface Z-direction length”; when the length of the part’s inclined surface is marked in the horizontal direction, R in the G10L12 program segment is “+#1-inclined surface horizontal length”.
5.2 Siemens CNC system programming example
When R1=Z preset value, R2=R1tan(tool tip angle/2)+(minor radius), the program is as follows.
TC_DP12[tool number, tool edge number]=-R1
TC_DP6[tool number, tool edge number]=R2
G0X25Y10
Z0
G01G41D(radius tool compensation number)X20F1000
Y0
G02X20Y0I-20
G01Y-10
G0Z50
When R1=contact radius, R2=[R1-minor radius]/tan(tool tip angle/2), the program is as follows.
TC_DP12[tool number, cutting edge number]=-R2
TC_DP6[tool number, cutting edge number]=R1
G0X25Y10
Z0
G01G41D (radius tool compensation number) X20F1000Y0
G02X20Y0I-20
G01Y-10
G0Z50
In the program, when the length of the part bevel is marked in the Z direction, the TC_DP12 program segment is “-R1-bevel Z-direction length”; when the length of the part bevel is marked in the horizontal direction, the TC_DP6 program segment is “+R1-bevel horizontal length”.
5.3 Okuma CNC system programming example When VC1 = Z preset value, VC2 = VC1tan (tool tip angle / 2) + (minor radius), the program is as follows.
VTOFH [tool compensation number] = -VC1
VTOFD [tool compensation number] = VC2
G0X25Y10
G56Z0
G01G41D (radius tool compensation number) X20F1000
Y0
G02X20Y0I-20
G01Y-10
G0Z50
When VC1 = contact radius, VC2 = (VC1-minor radius) / tan (tool tip angle / 2), the program is as follows.
VTOFH (tool compensation number) = -VC2
VTOFD (tool compensation number) = VC1
G0X25Y10
G56Z0
G01G41D (radius tool compensation number) X20F1000
Y0
G02X20Y0I-20
G01Y-10
G0Z50
In the program, when the length of the part bevel is marked in the Z direction, the VTOFH program segment is “-VC1-bevel Z-direction length”; when the length of the part bevel is marked in the horizontal direction, the VTOFD program segment is “+VC1-bevel horizontal length”.
5.4 Programming example of Heidenhain CNC system
When Q1=Z preset value, Q2=Q1tan(tool tip angle/2)+(minor radius), Q3=Q2-tool radius, the program is as follows.
TOOL “Tool number/tool name”DL-Q1 DR Q3
L X25Y10 FMAX
L Z0 FMAXL X20 R
L F1000
L Y0
CC X0Y0
C X20Y0 R
L Y-10
L Z50 FMAX
When Q1=contact radius, Q2=(VC1-minor radius)/tan(tool tip angle/2), Q3=Q1-tool radius, the program is as follows.
TOOL “Tool number/tool name” DL-Q2 DR Q3
L X25Y10 FMAX
L Z0 FMAX
L X20 RL F1000
L Y0
CC X0Y0
C X20Y0 R
L Y-10
L Z50 FMAX
In the program, when the length of the part bevel is marked in the Z direction, DL is “-Q1-bevel Z-direction length”; when the length of the part bevel is marked in the horizontal direction, DR is “+Q3-bevel horizontal length”.
6. Comparison of processing time
The trajectory diagrams and parameter comparisons of the three processing methods are shown in Table 5. It can be seen that the use of the forming angle milling cutter for contour programming results in shorter processing time and better surface quality.
The use of forming angle milling cutters addresses the challenges faced in end mill layer programming and ball cutter surface programming, including the need for highly skilled operators, reduced tool lifespan, and low processing efficiency. By implementing effective tool setting and programming techniques, production preparation time is minimized, leading to enhanced production efficiency.
If you wanna know more, please feel free to contact info@anebon.com
Anebon’s primary objective will be to offer you our shoppers a serious and responsible enterprise relationship, supplying personalized attention to all of them for New Fashion Design for OEM Shenzhen Precision Hardware Factory Custom Fabrication CNC manufacturing process, precision aluminum die casting parts, prototyping service. You may uncover the lowest price here. Also you are going to get good quality products and solutions and fantastic service here! You should not be reluctant to get hold of Anebon!