In recent years, with the development of digital control CNC processing technology, the processing center equipment with good performance has made the processing of many parts more convenient. How to use these equipment to efficiently process better quality parts has become a concern for enterprises. Taking typical thin-walled disc parts as an example, based on the advantages of high-speed machining and manufacturing technology applied in recent years, using the existing digital control CNC processing equipment in the factory, we actively explore better process plans and digital control CNC for processing such parts. Machining process.

    1. Process analysis of digital control CNC machining

    (1) The structural characteristics of the part The material of the part is duralumin LY12, which has good cutting performance. It is a typical thin-walled disk structure with a large external size. The thickness of the peripheral and internal ribs is only 2mm, and the cavity depth is 27mm. If the process plan or processing parameters are set improperly during the processing of the part, it is extremely easy to deform, causing the size to be out of tolerance.

    (2) Process analysis The part blank is selected from bar material, and the process plan of rough machining and finishing is adopted. The specific process flow is as follows: blank → rough turning → rough milling → aging → fine turning → fine milling. Rough turning: Reserve 1.5mm finishing allowance on the outer circle and end face respectively, and pre-drill the center hole. Rough milling: Reserve a margin of 1.5mm on the side and bottom of the cavity respectively, and pre-drill process holes at the φ12mm hole position. Aging: remove material and processing stress. Finish turning: Finish turning the end face, the outer circle and boring the process hole φ6mm, which requires one-time clamping to ensure the coaxiality and lay a good foundation for subsequent processing. Precision milling: to ensure the final requirements of the parts, is the focus of this article.

    ① Rough milling cavity rough machining mainly removes large margins and lays a good foundation for subsequent finishing. Therefore, when machining the cavity, choose a low-cost ordinary digital control CNC machining milling machine. This process requires machining the inner contour according to the shown part structure drawing, the arc corner is R5mm, and the remaining finishing allowance is uniform, 1.5mm. And this process also needs to pre-process the positioning holes required for finishing at the φ12mm hole position.

    ②High-speed machining technology of precision milling cavity is a manufacturing technology applied in recent years. In high-speed cutting processing, due to the small cutting force, the machining deformation of the parts can be reduced, which is more suitable for thin-walled parts, and the chips are removed in a short time, most of the cutting heat is taken away by the chips, and the workpiece is thermally deformed Small, it helps to ensure the accuracy of the size and shape of the parts; high-speed machining can obtain higher surface quality, and the machining cycle is greatly shortened. Therefore, in combination with the characteristics of this type of thin-walled disc parts, high-speed machining is selected when finishing the cavity.

    ③Machining of positioning holes The center hole φ6mm and φ12mm holes are used as positioning holes for the finishing of this part, so it must be machined in place before finishing the cavity. The center hole φ6mm will be bored to φ6H8 when the outer circle of φ301.5mm is precision turning; the φ12mm hole is drilled and reamed to φ12H8 by the digital control CNC machining milling machine.

    (3) Positioning and clamping of parts when finishing the cavity. In order to make the workpieces can be quickly and correctly clamped on the machine tool, and there is no need to align one by one when processing a batch of workpieces, so this processing adopts the positioning method of one side and two pins . Use the existing φ6mm and φ12mm holes on the part as positioning holes to make a simple tooling. The tooling uses a cylindrical pin and a flat pin as the positioning element. Since this part is a thin-walled part, it is easy to deform. When clamping the workpiece, the pressure plate should be pressed on the part of the workpiece with better rigidity, and the distribution should be as uniform as possible to ensure the reliability of clamping, and the clamping force should be appropriate. In order to prevent damage to the positioning of the workpiece or to produce unallowable deformation of the workpiece. Its specific positioning and clamping. This clamping method is fully in line with the characteristics of the machining center, and the cavity and all holes can be processed in one clamping.

    2. Digital control CNC machining program general plan for machining cavity

    (1) Programming software The numerical control CNC machining program of this part is generated based on the software MasterCAM. The software does not need to draw the entity, just draw the contour line to be processed correctly according to 1:1, select the appropriate graphics and parameters to generate the program for processing.

    (2) Selection of equipment Machining center equipment for finishing cavity selection: German HERMLE (Hammer) C1200U, the operating system of this equipment is HEIDENHIN (Heidenhain), and its performance indicators are: the maximum spindle speed is 18000r/mm, and the fast movement is 30000mm/ min, stroke 1200mm×1000mm×800mm, responsive, suitable for high-speed processing. This part has been processed by other machining center equipment before, but because of the thin wall, the rib thickness is only 2mm, and the cavity depth is 27mm. In order to prevent the part from deforming, only small-size tools and lower processing speed can be used. Many times of aging, the processing cycle is very long, so this processing uses digital control CNC processing equipment suitable for high-speed processing.

    (3) Tool selection According to the material of the parts, choose domestically-made carbide end mills with inserts, with large helix angle, large front space, wear resistance and low cost. After practice, it is found that the tool is very suitable for high-speed machining of aluminum. For the selection of specific parameters, you need to explore in actual cutting and find the appropriate speed. Of course, you must refer to the manufacturer's information.

    3. The finishing milling process of the machining center The milling of the cavity is carried out in two steps

The bottom surface and the side surface are processed respectively, the bottom surface first, and the side surface afterwards. The center of the digital control CNC machining program is set at the center of the outer circle of the workpiece, and the safety height is 50mm above the surface of the part.

    (1) Bottom surface machining tool specifications: use φ14mm end mills. Cutting method: The spiral cutting method can improve the cutting state during cutting, and maintain a higher cutting speed and lower cutting load. Cutting method: Choose Pocket-Parallel, Spiral, cleanCor-ners (parallel surround and clear corners) method, from the inside to the outside, the three cavities are processed separately, which can reduce tool lifting and improve milling efficiency. According to the down milling method, the machining allowance of 1.5mm on the bottom surface is completed in two times, the first tool back is 1.4mm, the tool path overlap is 50%, the speed is 8000r/min, the feed speed is 1400mm/min; during finishing , The amount of the back knife is 0.1mm, the speed is increased to 12000r/min, the feed is unchanged, and the surface quality of the bottom surface is very good. The tool path gradually expands from the inside to the outside, similar to the shape, the tool path is smooth and soft, and drastic changes are minimized to avoid vibration of the machine tool. Note: When finishing the bottom surface, 3mm margin is reserved for the side surface, so as not to increase the amount of cutting tool when milling to the side surface.

    (2) Side machining tool specifications: In order to prevent the sudden change of the tool path at the corner and cause too much impact, it is necessary to avoid the use of tools with the same corner radius during high-speed machining. This time, an end mill of φ8mm (corner R5mm). When installing the tool, shorten the extension length of the tool as much as possible to ensure the tool strength during high-speed machining. Tool advance and retreat mode: approach and leave the workpiece in a circular arc manner, which can avoid the tool mark caused by sudden contact with the workpiece and ensure the surface quality of the part. Feeding method: Contour (shape milling) method is selected. When machining, it is carried out in layers according to the Z axis and down milling. The speed is 10000r/min, the feed speed is 1000mm/min, and the three cavities are simultaneously milled down layer by layer, and the amount of back cutting is 2mm each time. Note: It is not possible to mill a cavity and then mill the next cavity. Because when the first cavity is processed, the wall thickness of the internal ribs is only 3.5mm, and when the next cavity is processed, the cutting amount of the internal ribs will be 1.5mm, which will cause the local supporting force to become smaller and the workpiece It is easily deformed by the influence of cutting force; if three cavities are milled down layer by layer at the same time, the wall thickness of the rib is 5mm, relatively speaking, the supporting force is much larger. After the machining operation of the machining tool path path is completed, select HEIDENHIN post-processing, generate NC program, and transmit it to the machine tool by network cable.

    Our products processed by CNC machining technology are suitable for automobile power amplifier heat dissipation, lighting heat dissipation, home audio heat dissipation, electronic heat dissipation and other industries.