Turning of Plug Valve Seats

Gas generators are widely used in metallurgy, building materials, the chemical industry, refractory materials, and other industries to provide mixed generator gas for their hot processing workshops. The structure of the gas generator is complex, and the flame detector is one of its important components. It is evenly distributed on the furnace cover or furnace body. The performance requirements of the flame detector components are as follows: When operating, the pressure in the furnace must be sealed to prevent gas from leaking; when not in operation, the sealing surface must maintain good sealing performance. To meet this requirement, the sealing cone surface between the plug valve seat and the valve core must have excellent sealing performance to ensure that gas does not leak. This requires that the processing dimensions of each seat part of the plug valve be highly precise, especially the cone hole that matches the valve core, which has extremely high precision requirements.
 

The plug valve seat must have precise processing accuracy and surface roughness, and the valve core and the valve seat cone hole must be ground to ensure that the sealing surface between the two has excellent sealing performance. The structure of the plug valve seat (Figure 1) is highly complex, making it extremely difficult to clamp and align on a lathe. The following is an analysis of these difficulties, in combination with the drawings.
 

Figure 1 The structure of plug valve seats
　　
As shown in Figure 1, the characteristics of the plug valve seat are as follows: First, the part has an irregular shape, and the external thread processing area is constrained by the 95×12 mm wheel-shaped outer circle on both sides. Ordinary thread tools cannot machine it, and a custom-made tool is required; second, the inner hole with a 30H7 tolerance and a 1:5 taper is 90 mm deep, with a surface roughness value of Ra=3.2 μm. The basic size and tolerance of the head are small, and the surface roughness requirement is stringent. Conventional tools are insufficient for completing the processing; third, processing the M27×1.5 thread in the lower inner hole makes it challenging to ensure accurate head clamping, necessitating the creation of a mandrel for proper positioning; fourth, due to the properties of ductile iron, uncontrolled cutting amounts can lead to burrs and scale fragments on the processing surface, affecting the surface roughness of the part; fifth, the part requires processing two fine threads, M48×2 and M27×1.5, with very small pitch and tooth height. Due to the material properties, improper control during thread processing can result in the thread teeth breaking.
 

To address these difficulties, the following measures are adopted after comprehensive consideration: First, the fitter should mark the plug valve seat as a whole, evenly divide the margin, and mark the cross center line and hole line in all directions to provide a reliable basis for lathe processing before turning it. The plug valve seat is processed on the horizontal C620 lathe. For a part with a complex appearance and high precision requirements, it is necessary to use self-centering chucks and single-action chucks for repeated clamping, strictly align with a mandrel, and create some special tools. Choose the cutting parameters to achieve high processing efficiency.

Use single-action clamping to process the upper M48×2 thread, the 30H7 inner hole, and the tapered hole for the first time. A single-action chuck is used for clamping. To facilitate alignment, a cross center line is drawn on the chuck jaw plane before clamping. Since the fitter has already marked the blank in the previous process, alignment in this step is straightforward: simply align the part's center line with the center line marked on the chuck. After alignment, the upper end face is turned using a standard method, followed by processing the 30H7 inner hole and the conical surface with a 1:5 taper, which presents one of the processing challenges. A custom-made inner hole turning tool bar (Figure 2) is used to address this difficulty. The tool bar is made from 45# quenched and tempered steel, with the rear part milled to a 25 mm×25 mm square for tool mounting. According to the drawing specifications, the hole depth is 90 mm, the conical surface depth is 50 mm, the taper is 1:5, and the maximum diameter is 30 mm. The front part of the tool bar is turned to a total length of 100 mm, with a straight section measuring 20 mm×50 mm, and a conical surface taper of 1:5. The front end of the tool bar is milled with a tool groove for welding a YG6 carbide tool head. This tool bar overcomes the disadvantage of ordinary turning tools, which are prone to vibration ripples due to their slender design. The tool head is welded to the center of the tool bar. There is sufficient clearance between the tool bar and the hole, allowing for smooth chip removal.
 

Figure 2 The turning tool
 
Before processing the tapered hole, use a 19 mm drill to pre-drill the through hole, and then machine the 30H7 straight section on the front end. When rough turning, set the speed to n = 280 rpm, the depth of cut to αp = 2.5 mm, the feed rate to f = 0.3 mm/rev, and leave 1 mm for fine turning. For fine turning, use a speed of n = 280 rpm and a feed rate of f = 0.15 mm/rev. Then, start machining the tapered hole. The tapered hole is machined using a manual small slide, and the scale line on the saddle is used to determine the size, turning it in 3 to 4 cuts. Finally, the groove is machined using the machine tool dial for alignment and feed adjustments. After machining, the tapered hole is ground and tested with a standard plug gauge. After machining the inner hole, proceed to cut the M48×2 thread, which is another challenging aspect of processing this part. At this stage, a special tool bar must be fabricated (see Figure 3).


Figure 3 A special tool bar

The front diameter of the tool bar is turned to 10 mm, the length is 30 mm, the end face is slotted, and the carbide cutter head is welded in place. It is essentially a special 90° left-biased tool, with the tool tip angle ground to 85°–87°. Both the outer circle and the thread can be machined in one pass with this tool. When machining the outer circle, use a speed of n = 180 rpm, a depth of cut of αp = 2.5 mm, and a feed rate of f = 0.28 mm/rev. When cutting the thread, note that the workpiece material is QT400-18, which is prone to chipping. Therefore, the cutting depth should be kept small. Although the pitch is only 2 mm, it must be machined in 5 passes. The depth of cut αp is set as follows: 1 mm for the first pass, 0.5 mm for the second pass, 0.3 mm for the third pass, 0.2 mm for the fourth pass, and 0.1 mm for the fifth pass. The speed should remain at n = 180 rpm to ensure the quality of the thread surface. After completing this process, the bottom surface needs to be machined.
 

Next, clamp the workpiece and machine the bottom end face and the M27×1.5 internal thread. At this stage, we encounter the fourth processing problem: how to quickly locate and align the workpiece to ensure the coaxiality of both ends. This problem can be addressed by using a mandrel. The inner end of the mandrel is aligned with the taper hole of the C620 lathe spindle, while the outer end is aligned with the taper of the workpiece's inner taper hole at a 1:5 angle. The inner and outer ends are connected using M30 standard threads, and locking nuts are provided for length adjustment. Note that the length of the tapered part of the positioning workpiece is 5 mm shorter than specified in the drawing to avoid interference during the processing of M27×1.5 threads. Automatic positioning is achieved by clamping the workpiece with the prepared mandrel. A single-action chuck is used for clamping. After machining the end face of the workpiece, proceed to machine the bottom hole. For machining, set the speed to n = 280 rpm, and machine the bottom hole in three passes. Then, use M27×1.5 standard taps to manually thread the holes, completing the processing of this end.
 

After processing the upper and lower ends, begin machining the left and right end faces and the 15 mm inner hole. Typically, parts of this shape are clamped with a single-action chuck, but alignment is complicated and inefficient. Here, we use a self-centering chuck to facilitate the alignment of the parts. Clamp one end of the part with the self-centering chuck according to the marked center line, align the other end to drill the center hole, and use the tailstock to support the workpiece while roughly machining the outer circle (it is sufficient to turn the circle). Next, rotate the head to clamp the outer circle that has been machined, align the center hole according to the line, machine the outer circle and end face to meet the drawing specifications, and drill the 15 mm hole. Rotate the head again to automatically clamp the machined end with the chuck, refine the center hole, machine the end face, and drill the 15 mm hole. In this manner, the 15 mm holes at both ends are machined in two operations and three clamping steps using the relative alignment method.
 

The machining of the plug valve seat on the horizontal C620 lathe was completed by fabricating two toolbars, designing the mandrel, selecting appropriate cutting parameters, and clamping the workpiece five times. Machining efficiency was enhanced by optimizing the alignment method and utilizing the self-centering chuck for clamping, which provided valuable experience for processing similar parts.