CNC machining technology of Large thin-walled hydraulic forged cylinder
For the thin-walled hydraulic forged cylinder CNC machining process focus and difficulties, respectively, from the machining method, cutting parameter optimization, tool selection, clamping, equipment selection, deformation control, etc., three types of typical parts features of the machining process for in-depth systematic analysis, and were proposed to solve the measures. After the actual processing verification, it eliminates the machining chatter phenomenon, improves tool durability, and ensures the parts’ surface quality and accuracy requirements.
Cylinder bore and wall thickness ratio D/δ ≥ 16 for thin-walled cylinder. Most of the cylinders at all levels of the vertical hydraulic forged cylinders in various aerospace models are thin-walled cylinders. The lifting hydraulic forged cylinder is a key component in each model, and its performance directly affects the performance and safety of the whole system. The cylinder structure shown in Figure 1 has high dimensional accuracy, roughness, and shape tolerance requirements.
Figure.1 Cylinder two-dimensional structure schematic diagram
Thin-walled cylinder barrel in the machining process is easy to deform, and the machining accuracy is more difficult to control; CNC machining brings great difficulty; this paper is mainly from the machining method, cutting parameter optimization, tool selection, clamping, equipment selection, deformation control, etc., the three types of typical parts features of the machining process for in-depth systematic analysis, and the development of specific machining programs.
2. Technical Program
Processing features mainly include the outer groove, inner groove, step surface, threads, etc.; the wall thickness is generally about 10mm, the width of the outer wide groove is about 25mm, the depth of deep grooves on one side of the depth is generally about 8-10mm.
The main process of cylinder barrel: rough turning – rough boring bore – heat treatment – rough turning – fine boring bore – semi-fine turning – fine grinding bore – fine turning – grinding cylinders – polishing.
This kind of parts in the process of machining, there are mainly the following difficulties and key issues.
- a. Cylindricity of the cylinder barrel is 0.05mm or less, which is not easy to ensure, and needs to be further optimized and improved in the machining process.
- b. The roughness of the inner and outer groove is Ra1.6μm, which is not easy to guarantee and needs to be optimized and perfected by the machining method, tool cutting parameters, and CNC machining toolpath trajectory.
- c. Cylinders at all levels are thin-walled cylinders with a large L/D ratio, which are prone to chattering and affecting the machining quality when turning the outer circle, so it is necessary to take anti-fibrillation measures and optimize the CNC machining trajectory; d. To ensure that the inner bore is Ra1μm, which is not easy to guarantee, optimizing the machining method, tool cutting parameters, and CNC machining toolpath is necessary.
- d. To ensure that the shape and position tolerance requirements of the bore, in the grinding of the bore, the roundness of the reference belt should be less than 0.01mm, and the need to optimize the processing of the reference belt is perfect.
2.1 CNC equipment, tool selection, and processing parameters
To ensure the machining accuracy of the parts, reduce the processing chatter phenomenon, and improve tool durability, the relevant equipment and process equipment put forward higher requirements: CNC equipment radial and axial runout should be less than 0.01mm, X and Z stroke should be able to meet the processing requirements of the parts; radial runout of the center bracket should be less than 0.003mm, the top of the radial runout should be less than 0.01mm.
Internal and external rough turning tool tip arc is recommended to use R0.8mm, precision turning tool tip arc radius is recommended to use R0.4mm; precision turning groove tool is recommended to use 3mm wide blade, combined with the actual processing, and based on the relevant tool samples, choose the appropriate groove type. The tempering hardness of the workpiece is generally HRC28-32; the actual verification and processing parameters are selected as follows.
Rough turning internal and external parameters: Vc = 110-118m/min, F = 0.22-0.25mm/r, ap = 2-3mm.
The parameters for fine-tuning are Vc=110-118m/min, F=0.1-0.12mm/r, ap=0.25mm.
Parameters of rough and finish turning inner and outer groove: Vc=90-100m/min, F=0.08-0.1mm/r.
Figure.2 Specialized customized toolholder
When machining the inner hole, the tool is easy to chatter. To improve the rigidity of the inner hole tool, some customized toolposts are needed, and then the tool is mounted on the toolposts, as shown in Fig.2.
2.2 Coordinate system selection requirements
The selection of the machining coordinate system pays attention to the following principles.
- a. The choice of coordinate origin as far as possible with the design and process reference overlap.
- b. The choice of coordinate origin should be convenient for numerical calculation.
- c. Coordinate origin should be selected in easy to find the right tool alignment, and in the process of machining is easy to check the position;
- d. Roughing zero points to choose the center of the two end faces.
- e. Semi-finishing and finishing in the processing of both ends of the inner circle, mainly selected in the center of the end face position; two top processing of the outer circle, to facilitate tool setting, coordinate zero point can be set at the root of the outer circle shown in Figure 3 position.
Figure.3 Coordinate position diagram
2.3 Typical feature machining method
2.3.1 Groove machining
There are two kinds of grooves in the cylinder barrel, namely, internal groove and external groove, and the roughness value of the groove bottom and groove wall is generally Ra1.6μm. When machining, it is necessary to formulate specific machining program according to the machining accuracy and the related roughness requirement, and the general requirements are as follows: for the thread backing groove, the overrun groove, and the oil groove with low technological requirements, it can be machined once in semi-finishing; for the demanding sealing groove, it should be machined by roughing, and then by machining with a different machining method. For high sealing groove requirements, the processing must be divided into rough turning, semi-finish turning, fine tuning, and other steps. Rough turning, slot wall allowance of 1mm, slot bottom allowance of 0.5mm; semi-finish turning and finish turning to ensure the cutting force maintains a basic constant; the feed rate should be converted to contour speed.
For groove roughing, you can use an alternate layering method for continuous turning; for each layer of the first cutting process, the feed will be reduced accordingly by about 25%; if the effect of the chip is not good, the use of intermittent processing. In processing shallow wide grooves, the first diamond-shaped tool is for semi-fine and fine-turning groove wall and groove bottom, and then use the groove knife or diamond-shaped knife reverse pick-up knife, as shown in Figure 4.
Figure.4 Wide groove semi-finish turning and finishing tool path schematic diagram
When machining narrow and deep grooves, finish turning the groove wall, then semi-finish turning the bottom of the groove, and finally lighten the groove wall and finish turning the bottom of the groove, as shown in Figure 5.
Figure.5 Narrow groove semi-finishing and finishing trajectory diagram
2.3.2 Machining of thread features
The threads in the cylinder barrel are metric threads with a 60° tooth angle. The machining quality of internal and external threads greatly influences the subsequent assembly, and the sharp edges of the threads should be obtuse. In order to meet the technical requirements of the premise, you can choose a variety of processing methods; specific requirements and methods are as follows.
- a. When processing threads, you can use a single thread cycle instruction G92 or composite thread cycle instruction G76 programming. The first knife processing depth is generally at most 0.6mm, gradually decreasing and, according to the actual situation, increasing the finishing or finishing tool path.
- b. Processing, it is recommended to use a fixed-pitch tool; due to different internal and external tooth types, internal and external fixed-pitch inserts cannot be mixed.
- c. After the completion of thread processing, should use the diamond-shaped tool, along the top of the tooth to the bottom of the tooth, to remove burrs flying edge, radial machining allowance of about 0.1-0.15mm, or the use of groove cutter, car to about 1/6 circle thread, specific should be based on the size of its pitch.
- d. Thread chamfer is generally 45 °; if the subsequent process needs to be used, it should be processed for 30 °, and its size should be more than the bottom diameter of the thread; the specific circumstances should also be in line with the relevant technical requirements.
- e. There are three main thread processing methods: straight into the method, oblique into the method, and alternating left and right processing methods, as shown in Figure 6. Straight into the method is suitable for processing pitch less than 3mm thread; G92 and G33 instructions are for straight into the processing of threads; for larger pitch thread processing, you can choose to slant into the method, G76 instructions that are slanting into the processing of threads; in addition, for thin-walled parts in the thread, to reduce the processing of the phenomenon of fluttering, the choice of alternating layers of processing, and the need to prepare a special processing macro program. With this method, a constant depth of cut can be realized, and the width of the cut is constant; during the machining process, the cutting force can be effectively reduced to maintain continuous steady state machining, tool life is high, and the machining quality is easy to ensure.
Fig.6 Thread turning method
2.3.3 Reference strip machining
When machining the cylinder barrel, it is necessary to finish the datum belt repeatedly. The machining accuracy of the datum belt will affect the machining quality of the subsequent processes, and the datum belt is shown in Fig.7.
Fig.7 Schematic diagram of datum belt
There are mainly the following processing methods for the datum.
- a. Precision requirements of the benchmark belt, you can use a clip as a top way to directly process into shape, such as for the deep hole boring process in the benchmark belt processing.
- b. High precision requirements of the reference belt can be used in two top processing, the specific process: first near the spindle side of the processing of a reference, and then turn around, in the spindle side of the processing of another reference belt, and accurate measurement.
- c. To meet the case’s processing accuracy, the benchmark belt’s high precision can also be used in a clip at the top of the processing. When processing, the tailstock pressure should be appropriately reduced, generally about 1MPa, and according to the actual equipment, to make appropriate adjustments.
2.3.4 Other Precautions
- a. After finishing boring is completed, the first receiving tool, if the deviation of the center axis of the bored bore is more than 0.25mm, four evenly distributed points should be selected, and the specific deviation value should be marked in the corresponding position, and then the spindle end of the refining cylindrical datum belt; b. In the two-top finishing boring, the tailstock pressure should be adjusted appropriately, generally about 1MPa, and adjusted appropriately according to the actual equipment.
- b. In the two top finishing cylinders, to reduce the chattering phenomenon, the inner wall of the cylinder barrel can be appropriately filled with cotton gauze, etc., and blocked with a round PE plate or support vibration-damping tooling in the inner wall.
- c. In the machining of grooves, easy to chatter phenomenon to solve the main measures: First, choose the appropriate tool and processing parameters; on the other hand, you can continuously adjust the method’s speed to reduce the chatter phenomenon.
3. Machining effect
Table.1 Comparison table of machining effect
|Item||Project||Before optimization||After optimization|
|1||Slot width size||Inconsistent size||All guaranteed, with high dimensional accuracy and good consistency|
|2||Thread surface quality||Tremor pattern||Eliminating chatter marks, achieving surface smoothness and meeting technical requirements|
|3||Machining chatter||Obvious tremor||Vibration elimination, smooth machining process|
|4||Tool life||Affected by vibration, low lifespan||Tool life increased by 25%|
The above comprehensive technical improvements have significantly improved the machining accuracy of threads, grooves, and reference bands. Adopting an alternating layering method to process threads eliminates the chattering phenomenon in the machining process and effectively controls the machining deformation. The groove wall finishing processing eliminates the phenomenon of groove broadband tipping; the specific effect is shown in Table 1.
By optimizing and perfecting the processing method of relevant features, optimizing the selection of tools, process equipment, cutting parameters, etc., the machining quality of the large thin-walled hydraulic forged cylinder is further improved to ensure the technical requirements of the product, which provides a successful example for the processing of similar products, and has a good value for promotion.
Author: Xu Junfeng