Innovative Process Refinement for Precision Cavity Machining
An efficient and cost-effective milling processing method was developed for a deep and narrow cavity part. The process was optimized based on the material and structural characteristics of the part. Improvements were made in the process flow, selection of milling tools, and processing parameters. Additionally, deep cavity corners were pre-treated, and a proper cooling method was implemented. These enhancements addressed issues such as vibration, difficulties in chip removal, and edge breakage during processing. As a result, tool life and processing efficiency were significantly improved, leading to reduced production costs.
PART. 01 Preface
Due to the characteristics of deep and narrow cavity structures, processing these parts requires tools with a larger aspect ratio. However, this approach can lead to issues such as vibration and chipping during machining. Additionally, challenges like poor cooling efficiency, difficulty in chip removal, reduced processing stability, low cutting efficiency, and shortened tool life arise. These factors contribute to the ongoing difficulties in processing and manufacturing.
PART. 02 Problems in part structure and processing
The structure and dimensions of a deep, narrow cavity part are illustrated in Figure 1. The material used for the part is 35 steel, forged, with overall dimensions of 100 mm × 100 mm × 220 mm. It features a corner with a radius of 8 mm and requires the machining of two grooves measuring 49 mm × 80 mm, each 200 mm deep, along with two side wall grooves.
During processing, it is essential to choose multiple tools with lengths exceeding 220 mm for both rough and fine machining. Due to the extended tool cantilever, vibrations during processing can be significant, increasing the risk of tool breakage. This also restricts the cutting depth and feed speed.
Moreover, as the milling depth increases, the effectiveness of cooling and chip removal decreases. This leads to a rapid rise in cutting temperature, which can result in tool wear and surface hardening. Consequently, this results in low cutting efficiency, a shortened tool lifespan, and poor surface processing quality. Given that this product is manufactured in large volumes, it is crucial to address these issues promptly to ensure processing quality, enhance efficiency, and reduce processing costs.
PART. 03 Processing technology optimization
The side wall of the component features square grooves measuring 30mm x 75mm and 30mm x 55mm. Additionally, the bottom of a φ46mm round hole includes a square groove measuring 40mm x 80mm, which leads to a deeper cavity. A φ40mm through hole is pre-drilled prior to the quenching and tempering processes.
Based on an analysis of the structural characteristics of the component, it is recommended that the two square grooves on the side wall, along with the pre-drilled φ46mm hole, be processed first to a diameter of φ45mm while reserving a finishing allowance.
This approach ensures that when the cutting tool reaches the depth of the square grooves and the round hole, it operates in an empty cut. This reduces the amount of material being cut, thereby increasing the tool’s lifespan and enhancing cutting speed. Furthermore, prioritizing the processing of the side wall’s hole grooves facilitates chip removal during CNC machining manufacturing, helping to avoid issues such as chipping and workpiece surface hardening that can arise when chips cannot be effectively discharged.
PART. 04 Selection of milling method
The inner cavity of the part is 200 mm deep, and it requires a significant amount of material removal from a hard material. To achieve efficient processing, it is crucial to select the appropriate milling method. After analysis, we determined that, since the workpiece is a quenched and tempered part with high hardness and a deep cavity, cycloidal milling and dynamic milling are not suitable options and can be excluded.
The plunge milling method (see Figure 2) offers distinct advantages for deep cavity processing and is one of the most effective ways to achieve a high material removal rate in metal processing. Its working principle involves changing the traditional horizontal feed to an axial plunge cutting technique, which transforms the cutting force from radial to axial. This allows for high processing rigidity, reduces vibration during the machining process, and enhances cutting stability, even with a large tool overhang.
During the plunge milling test, we observed that a wider cutting width increased material removal efficiency but also resulted in higher processing vibration, making the tool more prone to breaking. Conversely, reducing the cutting width led to lower processing efficiency and faster tool wear. Using ordinary alloy milling cutters for plunge milling resulted in shorter blade life and unsatisfactory processing outcomes; therefore, special plunge milling cutters are necessary.
Due to the considerable amount of cutting required for this workpiece, plunge milling is generally not feasible when preparation conditions are limited. However, if the parts possess good rigidity, a reasonable structure and material, and adequate preparation, utilizing special plunge milling tools can significantly enhance tool life and allow for efficient processing of deep cavity parts.
Under normal processing conditions and without the use of specialized plunge milling tools, conventional layered milling methods are more suitable for machining this part due to its structural characteristics. Before quenching and tempering, the workpiece should be pre-drilled with a 40mm diameter hole, which will serve as the cutting point for the milling process. Based on cutting experience with quenched and tempered steel parts, it is advisable to use a small cutting depth, along with a high speed and high feed rate, when machining this deep cavity. This approach will enhance processing stability and efficiency.
PART. 05 Corner pretreatment
When processing a deep and narrow cavity to its inner corner, the contact area between the tool and the workpiece increases significantly. This sudden increase in contact can lead to a sharp rise in cutting force, which may cause the tool to break or chip. To prevent this, it is advisable to pre-treat the corner of the cavity. One effective method is to use an extended drill bit that is slightly larger than the corner radius for pre-drilling, leaving a margin. This approach helps reduce both cutting force and cutting vibration at the corner.
PART. 06 Tool selection
(1) Tool Material Selection
When selecting tool materials for deep cavity milling, it’s essential that the tool exhibits excellent wear resistance and heat resistance, along with sufficient bending strength and toughness.
Among the commonly used cemented carbide tool materials in China, YG cemented carbide is known for its good bending strength and impact toughness, making it suitable for cutting brittle metals. YT cemented carbide, on the other hand, offers higher strength, wear resistance, and heat resistance compared to YG cemented carbide. However, its bending strength—particularly its impact toughness—is considerably lower, which makes it more prone to chipping.
YW cemented carbide combines high toughness, high hardness, and high wear resistance, effectively incorporating the advantages of both YG and YT cemented carbides. Utilizing YW cemented carbide can significantly enhance processing efficiency and overall processing quality.
(2) Tool Structure Selection
In deep cavity milling, several factors must be considered, including the number of teeth and the overhang length of the tool, as well as its rigidity, chip space, vibration, tool settling, and wear issues during processing. To ensure both strength and cutting efficiency, a high-feed end mill (see Figure 3) is recommended for rough milling. For fine milling of cavities and clearing corners, an indexable right-angle end mill (see Figure 4) should be utilized.
PART. 07 Optimization of processing methods
In the processing of deep cavity parts, the rigidity of the tool is proportional to the cutting amount. Increasing the rigidity of the tool can greatly improve the processing accuracy and processing efficiency.
1) Rough milling consists of two steps. First, a conventional high-feed end mill with a diameter of 32 mm (φ32 mm) is utilized, featuring a tool overhang of 115 mm and processing to a depth of 110 mm. Next, an extended high-feed end mill of the same diameter is employed, with an overhang of 205 mm, allowing processing to a depth of 110-200 mm. This approach significantly improves vibration and wear.
2) During the deep cavity processing, a conventional high-feed end mill and an extended high-feed end mill are used for rough machining. Subsequently, an indexable right-angle end mill is employed for fine milling of the cavity and for rounding the edges.
To address issues related to installation, manufacturing, and tool clearance errors during the rough milling process, it is important to note that the shank of the extended long-feed end mill may interfere with the machined slot wall, which measures 0 to 110 mm. To prevent this interference, the machining dimensions are adjusted by reducing the size by 0.1 to 0.2 mm compared to the first cutter. Finally, the indexable right-angle end mill is utilized for layered finishing of the cavity.
3) The tool path optimization process involves using a pre-drilled hole as the entry point for the tool. To ensure a smooth cutting operation, the arc tangent method is implemented for both entry and exit, which helps maintain a consistent cutting force without sudden changes. During the cutting process, the principle of “thick-in-thin-out” is applied, meaning that the chips are thicker when cutting into the workpiece and thinner when cutting out. This approach employs the down-CNC machining milling technique, effectively reducing tool vibration and extending tool life while also improving the quality of the slot wall surface. The optimized machining tool path is illustrated in Figure 5.
PART. 08 Optimization of cutting parameters
Cutting speed, cutting depth, and feed rate are the primary factors influencing cutting efficiency. Based on processing experience, cutting speed has the most significant impact on tool life. If the cutting speed is too low, it negatively affects processing efficiency; conversely, if the cutting speed is too high, it can shorten tool life. Next in line is feed rate, which also significantly affects tool life, while cutting depth has the least impact.
Methods for adjusting these parameters can generally be classified into two categories: using a large cutting depth with a small feed rate or a small cutting depth with a large feed rate. Cutting parameters can be adjusted within the ranges provided by tool manufacturers. For example, YW carbide mills can process tempered 45 steel parts at a cutting speed of 150-300 m/min, a feed rate of 0.15-0.3 mm/r, and a cutting depth of 0.3-1.2 mm. Given that cutting speed greatly affects tool life, it is advisable to make slight adjustments to this parameter while fine-tuning cutting depth and feed rate.
The results of adjusting the cutting parameters for tools with a large feed are summarized in Table 1.
According to the results presented in Table 1, using the “small cutting depth and high feed speed” method with this specific tool material and part material yields higher processing efficiency and longer tool life. The test cutting results indicate a high feed cutting speed of 181 m/min, a feed speed of 2500 mm/min, and a cutting depth of 0.8 mm. Under these conditions, cutting vibrations are significantly reduced, and tool wear remains normal. It is important to note that when utilizing an extended long feed tool, the feed speed should be reduced to 80% of that used with a standard tool.
PART. 09 Cooling technology
To improve efficiency in metal cutting, effective cooling is essential. Cutting heat impacts the formation and discharge of chips. Traditional cooling methods often have poor heat dissipation, leading to increased tool wear and reduced tool life.
High-pressure cooling cutting technology involves raising the pressure of the cutting fluid to a specific level and accurately spraying it onto the targeted cooling area for rapid cooling. This method allows the high-pressure cutting fluid to quickly remove chips, resulting in smoother machining, accelerated cooling, and extended tool life. Compared to standard cooling methods, high-pressure cooling can increase the tool feed speed and cutting depth within a limited range, thereby enhancing processing efficiency. The best cooling effect is achieved by combining high-pressure internal cooling with external cooling.
This processing uses a machining center without internal cooling, and adopts a combination of cutting fluid and high-pressure air cooling. During CNC machining processing, a large-flow cutting fluid pipe is used to aim at the tool tip to reduce the temperature and play a cooling and lubricating role. The air cooling pipe is aimed at the front end of the tool to quickly blow away the chips and ensure smooth tool processing.
PART. 10 Research results
A comparison of data before and after the test revealed that adjusting the processing parameters and optimizing the process flow can significantly enhance the efficiency of deep cavity processing. With all other parameters held constant, various cutting speeds, feed speeds, and cutting depths were tested. The results indicated that for rough processing using a large feed tool, the highest processing efficiency was achieved at a cutting speed of 181 m/min, a feed speed of 2500 mm/min, and a cutting depth of 0.8 mm.
The process flow was optimized by strategically arranging the workflow, selecting efficient tools, and implementing cooling technology. The data comparison revealed that the optimized processing method reduced processing time by 45%, increased tool life by 30%, and decreased downtime by 15%. This approach effectively utilized professional tools and equipment for processing deep cavity parts (see Figure 6).
PART. 11 Conclusion
This paper presents the development of a new milling method using a deep and narrow cavity part as a case study. This method addresses several challenges encountered during the machining process, including vibration, chip removal, and chipping. The research findings indicate that there is no single best processing method for metal machining; instead, the most suitable processing technologies and methods depend on the specific circumstances.
By optimizing the process flow, selecting appropriate tools and parameters, and implementing effective cooling measures, it is possible to enhance the efficiency of CNC machining of deep cavities, even with standard tools. Additionally, practical production considerations, such as workpiece clamping and equipment rigidity, must also be taken into account. The insights gained from this case study can serve as a valuable reference for improving the efficiency of deep cavity machining.
If you want to know more or inquiry, please feel free to contact info@anebon.com
Anebon’s commission is to serve our buyers and purchasers with the most effective, good quality, and aggressive hardware goods for Hot sale CNC prototyping service, aluminum CNC parts, and CNC machining Delrin made in China custom CNC machining services.