Selection of cutting parameters of TA15 and TB6 titanium alloy parts and tool technical parameters

The main machining method
    titanium alloy parts have a relatively large machining allowance, some parts are very thin (2～3mm), and the dimensional accuracy and shape tolerances of the main mating surface are relatively strict, so each structural part must be roughed → half The order of finishing → finishing is arranged in stages. The main surface is processed repeatedly in stages to reduce surface residual stress and prevent deformation, and finally meet the requirements of the design drawing. The main processing methods include milling, turning, grinding, drilling, reaming, tapping and so on.
    The amount of milling and the choice of tools
    are widely used in titanium alloy structural parts, such as the inner and outer surfaces of the parts. The cutting tool should choose materials with high hardness, high bending strength and toughness, good wear resistance, good thermal hardness, good manufacturability and good heat dissipation, mainly high-speed steel W6Mo5Cr4V2Al, W2Mo9Cr4VCo5 (M42) and cemented carbide YG8, K3O , Y330. The geometric parameters of the tool should be based on the principle of ensuring that the tool has high strength, good rigidity, and sharpness. The slenderness ratio should not be too large, and there are two types of roughing and finishing. It is best to use down milling during processing. The milling tool parameters are shown in Table 1, and the conventional processing and milling parameters are shown in Table 2. During milling, sufficient water-soluble oily cutting fluid must be injected to reduce the temperature of the tool and the workpiece, and the flow rate of the cutting fluid should not be less than 5L/min to extend the service life of the tool. On the basis of the above-mentioned conventional processing, in order to further improve the efficiency of milling processing, we conducted high-efficiency milling experiments on the powerful milling center machine tool, and obtained ideal cutting parameters, tools and cutting fluid. The data of milling parameters are shown in Table 3. It can be seen from the comparison between high-efficiency milling and conventional milling that the efficiency of high-efficiency milling processing is 2 to 4 times higher than that of conventional processing, the surface quality of parts is also greatly improved, the processing cycle is greatly shortened, and the manufacturing cost is correspondingly reduced.
    Turning amount and tool selection
    When the tool, cutting amount, and cutting fluid are selected reasonably, titanium alloy turning is not difficult, and it is close to processing alloy steel. However, it is more difficult to turn the surface oxide scale of titanium alloy. Generally, pickling is used to remove the thin layer of oxide scale on the surface before machining, and then the remaining oxide scale is turned. The cutting depth during turning should exceed the depth of the oxide scale by 1 to 5 times. Increase, but the cutting speed should be reduced. The tool material should be YG cemented carbide material. Tool geometry parameter selection: rake angle g0=4°～8°, relief angle a0=12°～18°, entering angle Ø45°～75°, blade inclination angle l=0°, tool tip arc radius r=0.5～ 1.5mm. Selection of cutting parameters: spindle speed n≥23Or/min, feed rate f≥0.10～0.15mm/r, cutting depth ap=1.5～2.0mm. When turning, sufficient water-soluble oily cutting fluid must be injected to reduce the temperature of the tool and the workpiece, and improve the durability of the tool. Table 1 Milling tool parameters. Tool rake angle g0
    (°)back angle a0
    (°)helix angle b
    (°) Tip tooth back Remarks End mill roughness O～412～1530～45 R-shape on demand b Large: smooth and precise cutting 4～815～2030～45 On-demand R-shape a0 Large: cutting force is small, machine vibration is small Three-face and face milling cutter 3～1012～15 On-demand end milling cutter 0～512～15 Entering angle Ø45°～75° Table 2 Conventional processing and milling parameters Tool material End mill diameter d
    (mm) Cutting speed V
    (m/min) Feed rate f
    (mm/min) Cutting depth ap
    (mm) Cutting width ac
    (mm) Cutting edge total length l
    (mm) Use machine tool K30≤2525～3550～1000.3～0.51.550～150 CNC machining center K30>2525～35100～1500.3～0.52.550～150 CNC machining center Table 3 High-efficiency machining and milling consumption Tool material End mill diameter d
    (mm) Cutting speed V
    (m/min) Feed rate f
   &nb
sp; (mm/min) Depth of cut ap (mm) Cutting width ac
    (mm) Total cutting edge length l
    (mm) Use machine tool K30≤2540～70200～3000.3～0.81.5～ 530～40 Power Milling Machining Center K30>2540～120 300～400 0.3～0.82.5～830～60 Power Milling Machining Center
    Grinding Quantity and Tool Selection
    Grinding can obtain higher precision, but it is determined by the unique properties of titanium alloy It is very difficult to grind titanium alloys. During grinding, the grinding wheel is severely worn, easy to become dull, and the grinding ratio is also low; at the same time, harmful tensile stress and serious surface burns are easily generated on the surface. Therefore, grinding should be avoided as much as possible and replaced by fine milling. Grinding material selection: Grinding titanium alloy chooses two kinds of abrasives: green silicon carbide (TL) and black silicon carbide (TH). If there is a tendency for grinding burns, synthetic diamond or cubic boron nitride grinding wheels should be used, which have good effects but are expensive. The hardness of the grinding wheel is softer, R3, ZR1, ZR2, and the particle size is 46 and 60, and type A bonding agent is selected. See Table 4 for the selection of grinding amount. Titanium alloy parts must be sufficiently cooled during the grinding process, otherwise the parts will change color or even burn. In addition to the cooling, lubricating and flushing effects of the grinding fluid, the more important thing is that it can effectively inhibit the adhesion and chemical reaction between the titanium and the abrasive. Table 4 Grinding amount Grinding method Grinding wheel speed v
    (m/s) Table speed V1
    (m/min) Workpiece speed V2
    (m/min) Grinding depth ap
    (mm) Transverse feed ①fa
    (mm/st) Longitudinal Feed ②fb
    (mm/r)
    (Wheel width B) Surface grinding coarse 15～1810～200.025～0.0350.5～4.0 fine 15～186～120.010 (maximum) 0.5～4.0 external cylindrical grinding 15～1815～300.025～O.0351/5B fine 15～1815 ～300.010 (maximum) 1/10B Note: ①Transverse feed fa (mm/st) refers to the amount of lateral movement of the worktable by the grinding wheel per single stroke of the worktable; ②Longitudinal feed fb (mm/r) refers to each rotation of the workpiece, The amount of longitudinal movement of the grinding wheel to the workpiece.
    Drilling amount and drill bit selection.
    Titanium alloy drilling materials should be selected with sufficient hardness, strength, toughness, wear resistance and low affinity with titanium alloys, mainly W6Mo5Cr4V2, W6Mo5Cr4V2Al, W12Cr4V4Mo, W2Mo9Cr4VCo5 and YG8, K30 Wait. The geometry of the drill bit should be noted: Table 5: Diameter of the helix angle of the drill bit with different specifications D: (mm) 2～66～1818～50 Helix angle b: (°) 43～4540～4235～40 Table 6 Drill diameter and external diameter The relationship between the relief angle af at the edge Drill bit diameter D: (mm) 2～66～1818～50 The relief angle at the outer edge af: (°)17～2015～1812～15 Table 7 The relationship between drill diameter D and inverted taper drill diameter D: (mm) 2～66～1818～50 Inverted taper: (mm/100mm) 0.03～0.050.04～0.080.05～0.12 Table 8 The relationship between drill diameter D and cutting amount Drill diameter D: (mm) spindle speed (r/min) Feed rate f(mm/r)≤3650～4500.04～0.063～6450～3500.06～0.116～10350～3000.07～0.1210～15250～2000.08～0.1415～20180～1500.11～0.1520～25120～900.12～0.20 Table 9 Reaming consumption Tool material Reamer diameter D
    (mm) Spindle speed n
    (r/min) Feed per tooth ar
    (mm) Reaming allowance (single side) ap
& nbs
p; (mm) M42≤10250～1200.02～0.04 Thick hinge: 0.10～0.15>10～20120～800.025～0.050 Fine hinge: 0.05～0.10 K30≤10800～4000.02～0.04 Thick hinge: 0.1～0.2>10～20400～ 2000.025～0.050 fine reaming: 0.05～0.10 appropriately increase the top angle of the drill bit, the top angle range is increased from 118°～120° to 135°～140°, the purpose is to strengthen the cutting part and increase the cutting thickness to improve the drilling effect. Choose a suitable helix angle b, the angle b increases, the rake angle also increases, the cutting is brisk, the chip removal is easy, the torque and the axial force are also small, see Table 5. Increase the thickness of the drill core to increase the strength of the drill bit. The core thickness is generally: K=(0.45～0.32)D, D is the diameter of the drill bit. Increasing the relief angle at the outer edge of the drill bit can sharpen the chisel edge and improve the cutting performance, especially for the drilling at the core of the drill. The selection of the relief angle at the outer edge is shown in Table 6. Machining into an inverted taper K can reduce the friction between the edge belt and the hole wall, reduce the torque when the drill is cutting, and improve the efficiency. The inverted taper is shown in Table 7. Drilling amount is shown in Table 8. It is best not to use chlorine-containing coolant when drilling and tapping titanium alloys to avoid the generation of toxic substances and hydrogen embrittlement. When drilling shallow holes, you can use electrolytic cutting fluid; when drilling deep holes, you can use N32 mechanical oil or vulcanized cutting. Reaming amount and tool selection
    Titanium alloy reaming is the last finishing process. Not only the productivity must be considered, but more importantly, the processing quality (precision and surface roughness) of the hole must be ensured. For this reason, the quality of the tool must be guaranteed, the cutting amount must be reasonably selected, and the coordination of the reamer and the drill and reaming die and the correct operation technology must be paid attention to. Through the processing method of drilling → reaming (rough reaming) → fine reaming, the requirements of product parts can generally be met. The tool material is generally M42 high-speed steel or cemented carbide K30. The geometric parameters of the tool are: rake angle g0=3°～7°, relief angle a0=12°～18°, entering angle Ø=5°～18°, blade angle l=0°. The width of the calibrated part blade band b=0.05～0.15mm, too wide is easy to bond with the titanium alloy processing surface, too narrow is easy to produce vibration during reaming. The number of reamer teeth Z=4～8 (the diameter of the reamer is Ø10～20mm). The ribs and joints processed by us have long spans and high coaxiality requirements. For this reason, lengthened drills and reamers are specially designed. The selection of cutting parameters is shown in Table 9. When reaming, the cooling lubricant should be continuously injected to obtain better surface roughness, and at the same time, chip removal should be performed frequently, and the chips on the reamer blade should be removed in time, and the knife should be advanced and retreated at a uniform speed during reaming.
    Selection of tapping amount and tool parameters
    Titanium alloy tapping will produce a large extrusion deformation, and the friction force acting on the thread side is increased, which not only makes the surface roughness of the processed thread not good, but also the tap is easy to break. In order to change this situation, you can use skipping taps or improve the tap structure (increase the clearance angle of the correction section teeth or increase the inverted taper) to reduce the cutting torque and friction torque, increase the chip space, and improve the tapping. The cutting performance of the wire. In addition, the diameter of the bottom hole before the titanium alloy tapping should generally be greater than the standard value, and the surface roughness of the bottom hole should reach Ra≤3.2μm. The tool material and geometric parameters are selected as the olive tap material. M2Al and M42 high-speed steel are selected. The geometrical parameters of the tap are: the rake angle g0=5°～8°, the back angle a0=8°～10°, the tooth back cylindrical land b1=0.1～0.2mm of the tap calibration section. Entering angle Ø6°～10°(through hole), Ø=15°～20°(without hole); nose cone Ø=2°～3°, double cone Ø=4°～5°. Cutting amount selection: The cutting amount of tapping is also only available as speed (rotation speed). The titanium alloy tapping speed v is 3-6m/min. When tapping, remove the burrs and chips at the tap edge in time to avoid damage to the thread; retract the tool frequently when tapping. Appropriate amount of cooling lubricant should be added when tapping, castor oil or engine oil is recommended to ensure the thread roughness requirements.