INFLUENCE OF TOOL PATH STRATEGIES ON MACHINING TIME USING THE BALL NOSE TOOL WHEN MILLING 3D SURFACES
Nhu Nguyet Vu* , Minh Tuan Ngo, Thuan Nguyen University of Technology - TNU
ABSTRACT
In machining flexible surfaces, machining processing costs can be reduced by several factors such as removed material workpieces, the choice of suitable cutting tools, optimal coolant and saving machining time. This paper proposes the effect of various toolpath methods for semi-finish operation on the machining time when milling 3D surfaces. An optimal selection of toolpath can cause remaking in the advance of time. The analysis and comparison of different toolpath strategies in 3D milling are investigated in order to choose the best strategies in different situations. The NX software, known as computer- aided manufacturing software, was used to evaluate the different toolpath strategies of three-axis milling. The experimental results clearly show the influence of the cutter path strategies on machining times and selecting the optimal strategy was based on a CAM software.
Keywords: Tool path strategy, machining time, three- axis milling, 3D surface, CAM software
Received: 29/8/2018; Revised: 13/10/2018; Approved: 28/12/2018
ẢNH HƯỞNG CỦA PHƯƠNG PHÁP CHẠY DAO ĐẾN THỜI GIAN GIA CÔNG KHI PHAY BỀ MẶT 3D SỬ DỤNG DAO PHAY ĐẦU CẦU
Vũ Như Nguyệt*, Ngô Minh Tuấn, Nguyễn Thuận Trường Đại học Kỹ thuật Công nghiệp - ĐH Thái Nguyên
TÓM TẮT
Trong gia công các bề mặt phức tạp, chi phí của quá trình gia công có thể giảm bằng vài cách như là lượng vật liệu phôi được hớt đi, lựa chọn dụng cụ cắt phù hợp, tiết kiệm dung dịch làm mát hay giảm thời gian gia công trên máy công cụ. Bài báo này đề cập đến hướng nghiên cứu ảnh hưởng của một số kiểu chạy dao trong khi phay bán tinh bề mặt 3D đến thời gian gia công. Việc chọn đường chạy dao tối ưu có thể dẫn đến những lợi ích nhất định cho thời gian gia công. Sự phân tích và so sánh các phương pháp chạy dao khác nhau khi phay mặt cong được đánh giá để chọn cách thức chạy dao tốt nhất trong nghiên cứu này. Phần mềm NX, được biết như là phần mềm trợ giúp cho quá trình gia công trên các máy công cụ, được chọn để sử dụng mô phỏng và so sánh sự khác nhau giữa các kiểu đường chạy dao khi lập trình phay 3 trục. Kết quả thí nghiệm cũng chỉ rõ ảnh hưởng của cách thức chạy dao đến thời gian gia công cũng như việc chọn được phương pháp gia công tối ưu trên phần mềm CAM.
Từ khóa: Phương thức chạy dao, thời gian gia công, phay 3 trục, mặt cong 3D, phần mềm CAM.
Ngày nhận bài: 21/9/2018; Hoàn thiện: 27/10/2018; Duyệt dăng: 28/12/2018
(*) Corresponding author:vunhunguyet@tnut.edu.vn; Tel. 0985960902
INTRODUCTION
In the milling processes using the CAD/CAM technology, the selection tool path strategy extremely affects the quality of machine parts and the machining time. By using a CAM software, the tool path and the way removing the material in the milling process can be simulated. Afterwards, having the verified accuracy as well as the efficiency of the operations, the CNC program is exported by input of the milling machine to produce the parts without confronting any problem of any kind. This, indeed, is another privilege of using computers in the production process, i.e., reducing machine time as well as reducing the production costs. The less the machining time, the cost of products decreases much.
In recent years, several studies have been conducted in optimizing the machining time parameters and the tool path strategies. In 2016, Mebrahitom A. studied the optimizing the tool path strategies and machining parameters for milling operations of a rectangular cavities [1]. In 2017, Bagci analysed the effect of tool path strategies on dynamic tool deflection, cutting forces, machining time, effective cutter diameter, cutter/workpiece engagement area, instantaneous material removal rate and machining errors in rough machining of a
sculptured surface [2].
Adriano Fagali de Souza focused on improvements on the choice of milling strategy in machining research and application [3]. Analysis of programming and simulations of manufacturing process in CNC milling machine applying through Mastercam software (CAD/CAM) were proposed by P.
V. Savalia and Prof. M. M. Chandrala [4].
The effects of cutter orientation used to machine curvature surface of thin aluminum parts (7075) with a 3-axis ball end-milling were investigated to improve geometric accuracy, surface integrity, and the most
optimal range of machining forces by B.
Jabbaripour [5]. A computation scheme that generates optimized tool path for five-axis flank milling of ruled surface was studied by Ping-Han Wu [6]. H. Perez proposed a machining strategy providing a cutting mode for the tool during a particular machining operation, determining the axial and radial depth of cut and the recommended trajectories for the cutting tool [7]. It can be seen that, several studies have been investigated to study the tool path strategies. However, influence of tool path strategies on machining time using the ball nose tool when milling 3D surfaces has not yet been reported. This paper presents the effect of various milling strategies for semi- finish ball end milling computer- mouse surface on the machining time.
SIMULATION CUTTING OPERATIONS WITH DIFFERENT TOOL PATH TYPES IN A CAD/CAM SOFTWARE
The models and drawings created by the designer have to undergo other processes to get to the finished product. Fig.1 shows the flow chart of the design and manufacturing process using a CAD/CAM software.
Figure 1. Design and manufacturing process using a CAD/CAM software
The process widely and commonly used to generate program codes for CNC machines to mill the component. This technological development reduces the amount of human intervention in creating CNC codes. After analyzing the geometry part, parent group objects are created to store manufacturing information such as tool data, feed rates, and tolerances, etc. The data is specified in the parent group object in inherited by operations that are listed under that particular parent group object. Usually, there are four types of parent group objects, such as geometry, method, program and tool. Before choosing operation types, numerous items must be taken into consideration for achieving the desired output.
In this work, the computer mouse surface is a complex surface and is designed on NX software as shown in figure 2. After creating the machining environment, the tool paths are created and generated for the cover housing.
Most of the CAM systems would provide for different area clearance options in which the user can choose considering the type of geometry. In NX software, there are 6 types of tool path strategies, such as the follow part, follow periphery, trochoidal, zig and zig zag.
The follow part is the most optimal strategy where the tool path manipulates depending on the part geometry. If there are cores and cavities in the part, the software will intelligently consider them to remove the materials in an optimal way. This kind of treatment is widely used for roughing operations. The follow periphery takes the path which depends on upon the periphery profile. For example, the outer periphery of our part is rectangular. So the tool path will be generated such that it gradually cuts the material from outside to inside with the step over value. This option is mostly used for projections and cores rather than cavities. The profile takes the cut only along the profile of the part geometry. It is used for semi- finishing or finishing operations. In the trochoidal method, the cutter is huge and is
used for removing a large amount of material.
The bulk of material is removed by gradual trochoidal movements. The depth of cut will be very high for this strategy.
Figure 2. The computer mouse surface model in NX software
Figure 3. The tool path strategies for the semi- finish milling process in NX software.
a) Follow part b) Zigzag c)Follow periphery d) Zig
The zig takes a linear path in only one direction of flow. In the zig zag method, the tool takes a zigzag path at every level of depth. It decreases machining time by reducing amount of air cutting time (idle running). The climb and conventional cuts alternate. These tool path types were used in this research. In this research, the free-form model was designed, and the machining operation was created in NX software as shown in figure 3. In this figure, the machining operations were designed with four tool path types in order to analyze the influence of the tool path strategies on machining time.
ANALYSIS RESULTS
After conducting simulation for different tool path types, the values of the machining time and the length of the NC program were calculated and recorded. Table 2 shows numerical values of the parameters for each of these strategies in the experimental tests.
Table 2. The numerical values of the parameters for each of these strategies in the experimental tests
The results are also shown in figure 4.
Regarding the simulated machining times, the shortest machining time belonged to the follow periphery strategy was 881 seconds because this can be found in the lowest movements of toward the safe level in Z direction and tool’s idle movement. The longest machining time, that is 218943 seconds with the zig strategy because of too many the non-cutting motions of the cutting tool.
EXPERIMENTAL WORKS
In this experimental study, the applied milling tool was a ball nose mill. The tool had a diameter of 8 mm and two insert flutes made from micro carbide and coated multi-layered
PVD when milling computer mouse surface C45 workpieces material. Experimental conditions were presented in table 3. The figure of actual operation of semi- finish mouse computer surface milling in Lab (Figure 5).
Figure 4. The machining time and the length of NC codes for the semi- finish milling process in
NX software
The experiment was performed in the Laboratory of Thai Nguyen University of Technology.
Table 3. Experimental conditions
Cutting tool P3202- WXM25
Design of cutting tool Ball nose mill Tool diameter d (mm) 8 mm
Flute (s) 2
Helix angle λ (◦) 15 Angle of rake γ (◦) −14
Coating Carbide with multi-
layered PVD Workpiece material C45
Hardness (HRC) 40 - 42 Binder
0,42% C; );15 % Si;
0,5% Mn; 0,025% P;
0,025% S; 0,2% Cr Machine tool Mazak VCS 530C Table Right/Left 1300 mm / 51.180 in Table Longitudinal 550 mm / 21.650 in
Spindle Taper 40
Maximum Speed 12000 rpm Number of Tools 30
Travel (X Axis) 1050 mm / 41.34 in Travel (Y Axis) 530 mm / 20.87 in Travel (Z Axis) 510 mm / 20.08 in
Table 4. Cutting parameters and machining time.
Tool path strategies
Cutting speed (m/
min)
Feed per tooth (mm/
tooth) Pick feed (mm)
Machining time
Zig 160 0.02 0.05 1h21'15"
Zigzag 160 0.02 0.05 56'09"
Follow
periphery 160 0.02 0.05 55'39"
Follow
part 160 0.02 0.05 1h21'13''
a)
b)
Figure 5. Some images of experiment a) Mazak VCS 530C. b) The part after miling.
CONCLUSION
This study investigated and compared the effect of three- axis tool path strategies on the free-form surface as the simulation of machining operation in NX software. Several remarks can be outlined as follows:
- The optimal tool path strategy for computer- mouse surface is the follow periphery method in three- axis milling aided by using NX software because the length of NC code is the smallest compared with others.
- The simulation shows that the machining time is speedy at the convex surface for the semi- finish milling when choosing the follow periphery method of the toolpath.
The experimental work shows that the machining time when milling using follow periphery tool path strategy is the smallest prepared with three different methods, it is mean that the optimal strategy for each geometry model was selected based on simulation in a CAM software.
ACKNOWLEDGMENT
The work described in this paper has been supported by Thai Nguyen University of Technology for ĐH2016-TN02-09 project.
REFERENCES
1. Mebrahitom A., Rizuan D., M. Azmir and M.
Nassif (2016), “Effect of High-speed Milling tool path strategies on the surface roughness of Stavax ESR mold insert machining, 114, pp 012006.
2. Bagci, Eyup; Yüncüoğlu, Ercüment U, (2017).
The Effects of Milling Strategies on Forces, Material Removal Rate, Tool Deflection, and Surface Errors for the Rough Machining of Complex Surfaces, Vol. 63 Issue 11, p643-656.
14p.
3. Adriano Fagali de Souza, Ernesto Berkenbrock, Anselmo Eduardo Diniz,
Alessandro Roger Rodrigues, 2015. Influences of the tool path strategy on the machining force when milling free form geometries with a ball- end cutting tool. Journal of the Brazilian Society of Mechanical Sciences and Engineering, Volume 37, Issue 2, pp. 675–687.
4. P. V. Savalia , Prof. M. M. Chandrala, 2017.
Generating Point Cloud Data by Using CMM for Surface Modeling and Select Proper Cutting Method to Optimize Total Machining Time.
Themed Section: Engineering and Technology, Volume 3, Issue 2, Print ISSN: 2395-1990,|
Online ISSN : 2394-4099, p826- 832.
5. Toh C. A study of the effects of cutter path strategies and orientations in milling. Journal of Materials Processing Technology. 2004 Oct;
152(3), pp. 346–356.
6. Wu, P.H., Y.W. Li, C.H. Chu, 2008. Optimized tool path generation based on dynamic programming for five-axis flank milling of rule surface. Machine Tools and Manufacture., 48(11), pp. 1224-1233.
7. Perez H, Diez E, Perez J, Vizan A. Analysis of machining strategies for peripheral milling.
Procedia Engineering. 2013 Sep; 63, pp. 573-581.
