Precision Side Milling Strategies for Single Cylinder Component Production

To address the issue of low rough milling efficiency for single-cylinder parts of hydraulic actuators, this text outlines the tool path, programming methods, and precautions associated with side milling these components. By analyzing the different milling types, process steps, advantages of side milling, and factors influencing the parts, we identify three rough milling techniques: milling additions, milling inner cavities, and milling the outer shape of single-cylinder parts. These methods collectively enhance the efficiency of rough milling for achieving the outer shape allowance.

 

01 Introduction

Hydraulic actuators are commonly used in aerospace and various other fields due to their excellent performance. They mainly consist of cylinders, pistons, and other components. The cylinder parts can be classified into three categories based on their structure: single-cylinder, double-cylinder, and complex-cylinder.

Single-cylinder parts (hereinafter referred to as cylinders) typically have a cylindrical shape, with oil pipes, oil pipe interfaces, and flanges located in specific areas. The manufacturing of these cylinders generally requires milling processing technology. Common examples of single-cylinder parts are illustrated in Figure 1.

 

Ordinary milling typically involves using a fast-feed milling cutter or an end mill and employs a contour milling approach to rough mill the outer shape allowance. This method is straightforward to program and easy to operate, demonstrating effective programming and processing techniques when the blank allowance is small and the shape is irregular.

However, in general, the height of the boss on a barrel shape is considerable, and using the ordinary milling method can lead to excessive layering in the height direction of the program, which ultimately results in low processing efficiency. This paper analyzes both ordinary milling and side milling methods for the barrel shape. It applies side milling to efficiently rough mill the outer shape allowance of the barrel, thereby enhancing the overall effectiveness of the rough milling process.

 

02 Process analysis

2.1 Types and steps of barrel milling

As illustrated in Figure 2, the milling processes involved in barrel processing are generally categorized into three types: milling addition, milling of the inner cavity, and milling of the outer shape. All barrels require the milling of the outer shape. When the raw material is a plate, a milling addition process must be included, while milling of the inner cavity is performed as needed based on the part’s structure.

In cases where the raw material is a plate, the blank has not been processed initially, and both the top and bottom surfaces are flat. The outer circle addition is roughly machined on the blank, which includes a two-dimensional milling addition process. If the cylinder wall features a large inner cavity structure, the blank has undergone pre-processing, with a flat top surface and a bottom surface that intersects with the inner hole of the cylinder. The inner cavity is roughly machined on the blank’s plane, and a two-dimensional milling inner cavity process is executed.

For parts that have a boss structure on the cylinder wall, the outer circle of the unbossed cylinder wall is turned to the dimensions specified in the drawing. Meanwhile, the outer circle of the cylinder wall with a boss is turned into a shape where one side is 1 to 2 mm larger than the boss. In this instance, a three-dimensional milling shape process is arranged. The milling methods for different material types are detailed in Table 1.

 

 

The milling process is divided into three steps: rough milling to remove the shape allowance, fine milling for precise shaping, and cleaning to eliminate any residual material.

Rough Milling of Shape Allowance: The goal of this step is to efficiently remove the shape allowance.

Fine Milling of Shape: This step ensures that the final dimensions match the specifications in the drawing and enhances overall processing efficiency.

Cleaning of Residue: The purpose here is to clean the root of the shape and remove any leftover material after fine machining.

Since rough milling of the shape allowance typically accounts for more than half of the total milling time, its efficiency significantly impacts the overall milling process. The milling steps are detailed in Table 2.

 

2.2 Advantages of side milling
Side milling is a processing method characterized by a large back cutting depth and a small cutting width. This technique offers several advantages, including high processing efficiency, increased feed rate, and extended tool life. These benefits arise from the effective use of the tool’s cutting edge.

In comparison to conventional milling, side milling’s smaller cutting width results in a shorter contact arc. This design prevents excessive heat transfer to both the tool and the workpiece, allowing for improved heat dissipation. Consequently, chips are discharged more efficiently, carrying away a significant amount of cutting heat and preventing it from concentrating at the tool tip. A larger back cutting depth enhances the effectiveness of the tool by maximizing the blade length used for cutting, which in turn increases the cutting edge’s efficiency and reduces overall tool wear.

In the context of barrel machining, side milling can be utilized in three main rough milling applications: barrel milling attachments, milling inner cavities, and milling outer shapes. Generally, the cutting width in side milling should not exceed 20% of the tool diameter. This limitation ensures a thinner cutting thickness and enables a higher feed rate. By using a larger back cutting depth, the side edge of the tool can be fully engaged, resulting in a higher metal removal rate and avoiding full cutting during processing. The differences between these two milling methods are illustrated in Figure 3.

 

 

2.3 Effect of tool diameter and overhang length on side milling

Side milling tools primarily utilize integral carbide milling cutters with extended cutting edges, ideal for the rough milling of contour allowances. The bottom of fast-feed milling cutters features a large radius blade, which can handle high-speed processing and heavy cutting conditions; however, the cutting edge of this tool is shorter, making it unsuitable for side milling of contour allowances.

Side milling is mainly employed for the rough milling of contour allowances, where processing accuracy is typically not a major concern. It is essential to use large-diameter tools that offer greater bending stiffness. By shortening the tool overhang length by 20% or increasing the tool diameter by 20%, the tool’s bending can be reduced by as much as 50%.

When selecting a tool, it is important to avoid situations where the cutting edge is excessively long or the diameter is too small. Additionally, it is advisable to minimize long tool overhangs during clamping. A smaller cutting width should be selected to prevent excessive bending or even breakage of the cutting tool. Based on experience, the back cutting amount should generally be less than or equal to two times the tool diameter.

For processing aluminum alloys, the cutting width should be less than or equal to 20% of the tool diameter. When machining stainless steel, high-temperature alloys, or titanium alloys, the cutting width should be limited to 7.5% of the tool diameter. Furthermore, the tool’s cutting edge length should exceed the maximum back cutting amount by 2 to 3 mm, while the tool overhang length should typically be 1 to 3 mm higher than the highest point of the part’s cutting top surface.

 

03 Side milling method of barrel

3.1 Tool path

When a part undergoes side milling, the back cutting can be substantial. This leads to a thin remaining blank when milling reaches the boundary of the part. Such a structure is prone to plastic deformation, which can cause springback and ultimately lead to chatter during the milling process. In more severe cases, these issues can result in tool breakage, destabilizing the process and preventing the proper milling of thin-walled parts.

The principle of thin-wall side milling is illustrated in Figure 4, while Figure 5 shows the part’s structure and Figure 6 displays the improved thin-wall design. During programming, the tool path is typically determined by the distribution of the part’s blank allowance, allowing for the selection of an appropriate thin-wall boundary to enhance the processing conditions as milling concludes.

 

 

When milling an attachment, the process typically begins with spiral milling from the outer edge to the inner center until the outer circumference of the attachment is fully milled. For milling the inner hole, a drill is initially used to create a pilot hole at the bottom, followed by spiral milling from the inside to the outer edge. When shaping the outer profile, it is common practice to start cutting from the arcs inwards and outwards to maintain the integrity of the remaining material. The three milling tool paths are illustrated in Figure 7.

 

3.2 Programming method

(1) 2D Contour Programming Method

When milling, Mastercam software is preferred. For milling inner cavities, CATIA software is the preferred choice. The process begins with using a twist drill or U-drill to create the bottom hole. Next, the plane feature command for outer milling is employed to cut from the center and mill outward gradually, step by step. The process of milling the inner cavity is illustrated in Figure 8.

 

(2) The 3D contour programming method is demonstrated using a cylinder, as shown in Figure 9, with the CNC custom machining profile feed path illustrated in Figure 10. When milling the profile of a part, two programming instructions are typically utilized: surface isoparametric line processing and curve-to-part processing mode.

For surface isoparametric line processing, it is essential to create the auxiliary surface in advance based on the blank shape of the part. Additionally, the initial path’s front extension must be set appropriately to ensure that the tool can gradually feed from the outside of the blank. As material is cut away, the tool feed path should extend outward from the blank, starting with a cutting allowance of zero.

In the curve-to-part processing mode, similar to the previous method, it is necessary to construct the auxiliary line or surface beforehand. The tool feed path should also be extended outwards from the blank according to the part’s blank allowance.

 

(3) Notes on Programming

When the A-axis of the part rotates, the cutting width at the lower section of the blank is denoted as ‘a,’ while the cutting width at the upper section is ‘a + δ.’ The greater the amount of back cutting, the larger the difference (denoted as 8) between the upper and lower cutting widths.

When programming, it is crucial to take the change in cutting width (8) into account to ensure that the cutting width of the tool does not become excessively large. The contour tool path for the surface isoparametric line machining is illustrated in Figure 11, while the principle analysis of this machining technique is presented in Figure 12.

 

4 Processing verification and application

4.1 Milling two-dimensional contour (milling addition)

The starting material for the cylinder is a plate measuring 500 mm x 130 mm x 230 mm. The process is designed to mill a cylinder with a height of 121 mm and a diameter of 128 mm on one end of the part. For the initial milling, a fast-feed tool with a diameter of 32 mm is used, resulting in a roughing time of 14.63 hours. For side milling, a 25 mm integral straight shank end mill is employed, with a roughing time of 7 hours. The parameters for the two-dimensional contour milling are detailed in Table 3, and the milling setup is illustrated in Figure 13.

 

 

 

4.2 Milling three-dimensional contour (milling shape)
The raw material for the cylinder is a bar measuring φ160 mm x 130 mm. The manufacturing process involves milling to create the desired shape. During the initial milling, a fast feed tool with a diameter of φ32 mm is utilized, resulting in a roughing time of 4.88 hours. For side milling the shape, a φ25 mm integral straight shank end mill is employed, which has a roughing time of 2.3 hours. The processing parameters for milling the three-dimensional contour of the cylinder are provided in Table 4, and an illustration of the milling shape can be found in Figure 14.

 

05 Analysis of processing effect

The limitation of back cutting depth results in the cutting length and axial back cutting depth in side milling being essentially the same. This leads to stable cutting forces, reduced surface roughness, and a significant improvement in processing efficiency. In ordinary milling, the chips produced are short and spiral-shaped, resulting in large fluctuations in cutting force and higher surface roughness.

In side CNC milling, the cutting occurs along the side edge of the tool. The resulting chips have a short, cylindrical disc spiral structure. Compared to ordinary milling, the contact arc in side milling is shorter, which minimizes heat transfer to the tool and the workpieces. Additionally, the larger heat dissipation space of the tool helps manage heat more effectively.

The small cutting width in side milling produces smaller and shorter chips, facilitating smooth chip discharge. This helps to remove a significant amount of cutting heat and extends the tool’s service life. The chip shape is illustrated in Figure 15, while the tool wear is depicted in Figure 16.

 

06 Conclusion
This study analyzes the machining process and characteristics of rough milling for single-cylinder components in hydraulic actuators. A targeted machining scheme for side milling the outer shape allowance was proposed. Three different approaches to rough machining were implemented: milling of single-cylinder extensions, milling of inner cavities, and milling of outer shapes. This approach achieved efficient rough milling of outer shape allowances. We presented a relatively advanced and practical milling technology specifically designed for single-cylinder parts, which provides effective guidance for improving similar components in subsequent processes.

 

 

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

OEM/ODM Manufacturer China Casting and Steel Casting, The design, processing, purchasing, inspection, storage, and assembling process are all in scientific and effective documentary process, increasing usage level and reliability of our brand deeply, which makes Anebon become a superior supplier of the four major product categories, such as precision CNC machining parts, CNC milling parts, CNC turning and metal die casting service.