Precision Turning Techniques for High-Strength Steel Fan Shafts

Based on the material properties and the challenges associated with machining the fan shaft, a suitable turning process route has been developed. Enhancements have been made in several areas, including material heat treatment, part clamping methods, tool selection, thread processing programming, and processing parameters. These improvements ensure processing accuracy while addressing the turning challenges posed by high-hardness materials, ultimately reducing tool wear.

To tackle chip entanglement during the cutting process, we calculate the cutting depth for each feed and the rotation angle of the part. An alternating forward and backward chip-breaking scheme is implemented on the CNC lathe to effectively resolve this issue.

 

01 Preface

Among the various components of an aircraft engine, the high-strength steel fan shaft is a crucial part of the fan unit. This component operates under extreme conditions, including high speeds and elevated temperatures, and is responsible for transmitting torque between the engine units. The quality of the shaft’s surface, its accuracy, roundness, circular runout, cylindricity, coaxiality, and positioning significantly affect the engine’s functioning, longevity, and safety. Therefore, it requires very high dimensional accuracy.

The material used for the shaft is 00Ni18Co8Mo5TiAl, a high-alloy high-strength steel that achieves a final hardness exceeding 48HRC. This material is considered challenging to machine due to its poor thermal conductivity, tendency to produce burrs, good toughness, and susceptibility to chipping. To achieve high machining efficiency while ensuring consistent quality, it is essential to optimize the turning process, tool selection, and machining parameters for the fan shaft.

In Figure 1, a cross-sectional view of the high-strength steel fan shaft is presented. The outer surface features a multi-step ladder structure. The diameter tolerances for all mating components range from 0.015 to 0.026 mm. Both axial and radial runouts are required to be within 0.015 mm, with tolerance grades in many areas falling between 6 and 7.

The shaft is made from 00Ni18Co8Mo5TiAl material, also known as C250 steel, which is classified as high-alloy, high-strength steel. This material exhibits notable characteristics, including high elongation, cross-sectional shrinkage, and impact values, which set it apart from general steel in terms of cutting performance. The main characteristics that affect processing are as follows:

1) The material has a very high hardness of ≥48 HRC, making it challenging to cut.
2) It possesses good toughness but strong chip adhesion, which leads to the entanglement of chips and makes it difficult to break them.
3) The material has low thermal conductivity, meaning cutting heat cannot dissipate quickly, resulting in the cutting edge of the tool overheating. As the cutting speed increases, the temperature rise becomes more pronounced, causing the tool to wear out faster and lose its cutting effectiveness.

Several issues must be addressed when processing parts:

1) From the perspective of the process route, it is essential to tackle the challenges posed by high material hardness and difficult turning while ensuring processing accuracy.
2) From the tool standpoint, it is important to ensure efficient processing and mitigate excessive tool wear.
3) Regarding chip breaking, solutions must be found for the material’s tendency to easily entangle chips.

 

03 Process route

3.1 Solution treatment and aging treatment

To address the issue of high material hardness, it is advisable to begin with a solution treatment on the blank to reduce its hardness and eliminate any large excess material. Start by heating the material to a temperature of 820±10°C and maintain this temperature for 1 to 2 hours. This step ensures that the alloy elements in the steel dissolve fully into the iron matrix, forming a uniform solid solution and promoting grain growth, which in turn reduces the material’s hardness.

Once the solution treatment is complete, allow the material to air cool to room temperature to achieve a hardness level below 34HRC. This reduction in hardness will enhance the efficiency of the subsequent rough turning process, during which the excess material is removed.

After the large excess has been turned away, proceed with the aging treatment. Heat the material to 480±6°C and maintain that temperature for 3 to 6 hours, followed by air cooling to room temperature. The aim of this step is to control the cooling rate and temperature to decompose the supersaturated solid solution and precipitate the hardening phase, increasing the hardness to at least 48 HRC to meet the desired final state. Finally, conduct a finishing operation to remove any small excess and ensure accurate dimensions.

 

3.2 Turning datum

The roundness, cylindricity, coaxiality, and surface roughness of parts significantly impact the rotational accuracy and operational stability of the shaft. Therefore, establishing a turning datum is a crucial step in the machining process. The flatness of the part’s datum surface directly influences the accuracy of subsequent dimensions, as well as the positional accuracy of the axial hole and the overall profile.

The clamping method used during the turning process is illustrated in Figure 2. Initially, the radial runout of the W and X datums is aligned to within 0.01 mm. Following this, the outer surface of the part is turned, and the center hole of the small end’s inner hole is refined. This process establishes an alignment datum for subsequent operations.

 

3.3 Finishing the inner and outer surfaces of the large end

The clamping method used for finishing the inner and outer surfaces of the large end of the part is illustrated in Figure 3. A self-centering chuck is employed to secure the surface that was processed in the previous operation, aligning the radial circle runout of the outer diameters, C and W, at both ends of the part to within 0.005 mm. Additionally, a center stand supports the outer circumference of the large end, establishing the axis of the part and ensuring that the workpiece’s rotation axis is aligned with that of the machine tool.

To prevent the workpiece from bending or deforming due to cutting forces and its own weight, a hydraulic center stand is positioned to support the outer cylindrical surface adjacent to the large end. Furthermore, to prevent axial movement of the part, a pressure plate is used to secure it at the step of the workpiece. This clamping method is capable of withstanding greater cutting forces.

Once the part has been processed, the axis is effectively corrected, allowing for the completion of the large end face in a single clamping. This method ensures the verticality of the end face relative to the axis and maintains reliable clamping for subsequent operations.

 

3.4 Finish turning the inner and outer surfaces of the small end

The clamping method of the parts when finishing the inner and outer surfaces of the small end is shown in Figure 4.

 

Once the cast iron faceplate is installed on the machine tool spindle, it is turned and trimmed to ensure that any fixtures mounted on the faceplate are perpendicular to the machine tool’s axis. This process guarantees that the part’s axis aligns with the machine tool’s axis. The large end of the part is supported by the mounting edge, with the inner stop of the large end used for positioning. The back of the mounting edge is pressed tightly, and the center frame provides additional support. The radial runout of the X and W parts should be aligned within 0.005 mm. The total length of the part and its inner cone are then turned. Without disassembling the center frame, the part’s inner hole is supported at the center, and the front face is checked to ensure it matches the pre-processing position. This method, known as the “one clamp and one support” scheme, is employed to process the part’s outer circle.

After machining the outer cylindrical surface, the part’s surface near the small end is first supported by the center frame. Once this is done, the cone plug is removed, and the “one clamp and one support” method is again utilized to process the characteristic surfaces of the part’s inner cavity. This approach effectively ensures that all turning surfaces align with the machine tool’s rotary axis.

To improve processing efficiency, a cutter is used to remove excess material from the large areas of the inner and outer circles. Finally, an R cutter is employed for profiling the parts. To ensure accurate sizing of the intersection at the bevels, a specialized tool calibration program is set up while compiling the CNC program. This calibration determines the precise values for the X and Z directions of the parts, followed by polishing to ensure high processing accuracy.

 

3.5 Processing of high-precision threads

The outer diameter of the fan shaft features a left-hand sawtooth thread measuring M196 × 1.5, a triangular thread measuring M155 × 1, and another triangular thread measuring M118 × 1.5 (refer to Figure 5). The threading process is carried out on a lathe using forming tools. The quality of the thread blade’s grinding has a direct impact on the overall quality of the threading operation. It is important that both the left and right cutting edges of the turning tool are straight lines, the tip angle of the blade matches the tooth angle of the thread, and the cutting portion of the thread blade maintains a low surface roughness value.

 

When programming a CNC lathe, the “radial feed” method is utilized for threading operations. In this method, the blade is fed vertically, completing the thread processing through several strokes. Chips generated during cutting are discharged either perpendicular to the axis of the thread or rolled up and ejected. If an axial or oblique blade is used, the high-speed discharged chips can roughen the opposite side of the tooth. This technique allows for achieving a relatively accurate tooth profile with high precision.

Different instructions are employed for various types and sizes of threads on the CNC lathe. For M196 threads, the “G32 thread cutting” command is used, with a serrated thread blade produced by Stram selected for processing the components. With serrated left-hand threads, it is important to note that the thread profile is self-locking. When measuring these threads with a thread ring gauge, if it feels tight, you must slowly unscrew it in the opposite direction; failing to do so could damage the thread and lead to scrapping the part.

For triangular threads, the “G76 thread cutting” command is appropriate on the CNC lathe. Analysis of the programs compiled for the two different thread specifications shows that the thread profile angle remains consistent; however, variations exist in the starting point, end point size, and pitch. When programming, it is crucial to accurately specify the thread profile angle and pitch; otherwise, defective products may result.

During thread turning, the feed rate of the machine tool is the most critical factor, as it must match the pitch of the thread. This requirement means that when using a profile insert for thread cutting, it’s essential to maintain a high feed rate and cutting speed. The synchronization between feed rate and pitch can be managed through the solidification subroutine of the CNC machine.

In thread turning, the profile insert can perform the necessary number of passes along the workpiece to produce the desired thread. To avoid overloading the thread profile angle of the cutting edge while preserving its sensitivity, the total cutting depth of the thread should be divided into several smaller cutting depths. As each pass is made, a portion of the total cutting depth is removed. As the insert cuts deeper, the axial feed value will gradually decrease, allowing the cutting edge to engage more deeply and generate additional threads.

To determine whether the thread is acceptable, a serrated thread ring gauge is required. During actual measurement, fine chips and dirt on the thread can interfere with the accuracy of the gauge, so it’s important to use a metal eraser to remove fine chips and clean the parts with alcohol before using the thread ring gauge.

 

04 Reasonable selection of tools and processing parameters

After rough machining and solution treatment of the fan shaft, a margin of 3.3 mm is reserved in certain areas to prevent deformation during heat treatment. Initially, the conventional processing method illustrated in Figure 6 was adopted. The tool used is a CNMG120408-PM4225, which is a classic C-type tool known for its high processing efficiency. The cutting depth ranges from 1.2 to 1.5 mm, with a cutting speed of 120 m/min and a feed rate of 0.15 mm/rev. Typically, this step takes about 1 hour to complete. Upon finishing the machining process, the cutting edge of the tool exhibits noticeable wear.

 

After analysis, it was determined that the fan shaft utilizes a “one clamp and one top” positioning method during the processing of the outer circle. This method ensures stable positioning, and given the part’s thick walls and good rigidity, both the cutting speed and rotation speed, as well as the cutting depth, can be increased to enhance processing efficiency. However, the potential for efficiency improvement using conventional tools remains limited.

Ceramic inserts are often favored for boosting processing efficiency, but their design constraints make them more suitable for simpler shapes. When processing stepped surfaces, there tends to be a significant remaining margin at the corners, requiring considerable time to clean up the roots, making them less ideal for fan shaft processing.

Following a thorough evaluation, we recommend considering a new alloy tool from Sandvik Coromant for high-speed machining. This tool features a design that falls between C-type and V-type tools, with a long blade length and superior strength thanks to double main deflection angles compared to V-type tools. During reverse turning, the smaller main deflection angle enhances tool strength, and the larger side blade contact area improves heat dissipation.

 

Testing showed that, under unchanged cutting depth conditions, the cutting speed can be increased to 140 m/min, with a feed rate reaching 0.9 mm/r. This results in completing this step in just 12 minutes, significantly reducing the processing time for semi-finishing the outer circle. The machined surface, although exhibiting a relatively high surface roughness of Ra ≈ 3.2 μm, retains a margin of about 0.3 mm on the surface, which does not impact the final quality.

The cost of the new blade is approximately three times that of the original blade, but it also lasts three times longer. In conclusion, this approach effectively meets the goals of high-efficiency processing while ensuring quality, and this empirical method can be promoted for use with shaft and disk parts that exhibit good rigidity.

 

05 Use chip breaking solutions to solve the problem of chip entanglement

The fan shaft material exhibits good toughness, which results in the semi-finished grooves producing continuous and curled chips. These chips tend to entangle with both the workpiece and the center frame, leading to scratches on the processed surface and significantly impacting the quality of the machining. Some of these entangled chips can obstruct the cooling of the cutting area by the cutting fluid, potentially causing tool damage. Additionally, entangled chips can interfere with the proper positioning of the center frame, which may result in radial runout, axial runout, or chipping of the product.

Currently, the only method to manage this issue during processing is through manual observation and cleaning of the chips. At times, it becomes necessary to halt the machine to clear the chips, which is both risky and inefficient. Therefore, it is crucial to address the problem of chip entanglement using effective chip-breaking techniques. The conventional chip-breaking methods include the following:

1. Utilizing a chip breaker or chip-breaking device, which is often not economical and inconvenient to install.
2. Selecting tools with different chip-breaking grooves. However, the challenge lies in accurately matching the geometric parameters of the tool with the processing part and material. Various chip breaker tools with different shapes have not yielded satisfactory chip-breaking results when machining the fan shaft. Furthermore, simply increasing the front angle of the chip breaker compromises its wear resistance, preventing the successful completion of the machining process.

 

3) Pecking machining involves frequently and periodically changing the cutting depth during the machining process. This results in intermittent chip generation, which prevents chips from becoming entangled, thus addressing the chip entanglement issue. However, in conventional pecking machining, the timing for tool withdrawal is often set arbitrarily, making it challenging to control chip length, particularly when machining larger diameter parts. If the chips are too long, they can still become entangled, while chips that are too short may scatter uncontrollably.

To enhance this process and improve chip length control, further refinements can be implemented. By calculating the cutting depth for each feed in relation to the part’s rotational angle during CNC process, it is possible to determine the relative displacement length caused by the tool cutting in and out of the part’s surface. This calculation involves the angle of rotation of the part per unit of time, allowing for better control over chip length. The principles of this improved pecking machining method are illustrated in Figure 10.

 

Using this principle, the machining program was rewritten in combination with the machining parameters of C250 material. The calculation formula for the time t taken by the tool to turn the workpiece surface once is
t＝60πD/（1000vc）（1）

Wherein, t is the time taken by the tool to turn the workpiece surface once (s); D is the diameter of the workpiece processing part (mm); vc is the cutting speed (mm/s). The calculation formula for the back cutting amount ap of each feed after setting the chip length is
ap＝Lfnt/（60πD）（2）

Wherein, ap is the back cutting amount of each feed after setting the chip length (mm); L is the required chip length (mm); f is the feed rate (mm/r); n is the spindle speed (r/min); t is the time taken by the tool to turn the workpiece surface once (s); D is the diameter of the workpiece processing part (mm).

The coordinate points of the tool trajectory are compiled to create a machining program that processes one cut after another until the specified depth is reached. Each feed coordinate point differs from the previous one by a back-cutting amount, denoted as “ap.” Similarly, each retract coordinate point also differs from the previous one by the same back-cutting amount, “ap.”

For example, if the coordinate point on the surface of the part to be processed is X0, then the first feed coordinate point (X1) will be X0 – ap, the second coordinate point (X2) will be X0 + ap, the third coordinate point (X3) will be X2 – ap, and so on, continuing in this manner until the specified depth is achieved. Additionally, the relationship between the back-cutting amount and the angle of axis rotation is illustrated in Figure 11.

 

It has been confirmed that when chips are generated consistently and arranged in a “pagoda shape,” they do not become tangled or splash around. This effectively addresses the issue of chip entanglement. Figure 12 illustrates the difference between the original chips and those processed using the improved procedures.

 

 

06 Conclusion

This article discusses the CNC turning process for high-strength steel fan shafts. It focuses on optimizing and improving the process route, cutting tools, and processing parameters. The aim is to address the challenges associated with turning high-hardness materials, such as chip entanglement and tool wear. The results demonstrate that this turning process not only ensures high quality and quantity but also achieves excellent turning efficiency and precise dimensional accuracy. Additionally, the approach effectively resolves the issue of chip entanglement. The chip-breaking methods and processing tools presented in this article are also applicable to the machining of other similar materials.

 

 

 

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

Anebon has numerous great personnel members who are good at advertising, QC, and working with troublesome dilemmas from the creation course of action for China Supplier. High Cost-Effectiveness 5 axis CNC machining parts, milling aluminum parts with high-speed machining and high pressure aluminum die casting parts.