Take the example of No. 45 steel with a blank size of 100mm×100mm×30mm and processed to a thickness of 25mm.
Clamping of Workpiece
When milling a plane, the workpiece’s machined surface must be higher than the jaws, otherwise the workpiece must be raised with parallel shims to expose enough machining allowance to avoid damaging the jaws. In order to clamp firmly and prevent the workpiece from loosening during milling, the plane that is close to the shim and the jaws must be cleaned. To make the workpiece close to the shim, it should be clamped while tapping the surface of the workpiece with a hammer. The machined surface should be tapped with a copper rod to prevent scratching the surface and affecting the quality. Move the shim by hand to check the degree of clamping. If it is loose, it means that the workpiece and the shim are not well fitted, and the flat-nose pliers should be loosened and re-clamped.
Choice of Milling Cutter
According to the tooth density, face milling cutters are divided into three categories: low density, medium density, and high density. The density of the inserts of dense-tooth milling cutters is too high. The more blades enter the workpiece at the same time, the greater the machine power required. Moreover, it may not be able to ensure sufficient cutting clearance, so that the chips cannot be discharged in time and block the cutter, so it is often used in finishing occasions with small cutting volume. The most important point of plane milling is the selection of the diameter size of the face milling cutter. For one-time plane milling, the ideal width of the plane milling cutter should be 1.3 to 1.6 times the width of the material, so as to ensure the good formation and discharge of chips. Since the plane size of the processing is 100mm×100mm, the size is relatively large, and a four-piece small density machine plus face milling cutter with a diameter of 60mm is selected here for processing.
Determination of Processing Trajectory
When determining the processing trajectory, the following situations should be noted:
If the workpiece only needs one milling, the tool center trajectory should be avoided from coinciding with the center line of the workpiece. When the tool center is at the center of the workpiece, it is easy to generate vibration, resulting in poor processing quality. Therefore, the tool center trajectory should deviate from the center line of the workpiece.
When the tool center trajectory coincides with the edge line of the workpiece, the impact force of the cutting insert when entering the workpiece material is the largest, which is the most unfavorable situation for tool processing. Therefore, the tool center line should be avoided from coinciding with the edge line of the workpiece.
If the tool cuts into the workpiece less than half, when it just cuts into the workpiece, the impact speed of the blade relative to the workpiece material is large, causing a large collision force, which is easy to damage the tool or produce a gap. Therefore, when planning the tool center trajectory, it should be avoided that the tool cuts into the workpiece less.
When the tool cuts into the workpiece more than half, the insert that has cut into the workpiece material bears the maximum cutting force. The insert that has just cut into the workpiece is subjected to less force, causing less collision force, which can extend the life of the insert. Therefore, it is usually necessary to try to keep the center of the face milling cutter in the workpiece area, and avoid the overlap of the tool center and the workpiece center when the workpiece only needs one cut.
When milling a large area of workpiece plane, multiple milling is the most commonly used method, which can be divided into unidirectional multiple cutting and bidirectional multiple cutting at the same depth. In unidirectional multiple cutting, the cutting start point is on the same side of the workpiece, and the other end is the end point. After each cut, the tool returns to the cutting start point from above the workpiece. This is a common method in plane milling. Frequent rapid return motions result in low efficiency, but it can ensure that the face milling cutter is always milling forward. Bidirectional multiple milling is also called Z-shaped milling, and it is also frequently used. Its efficiency is higher than that of unidirectional multiple cutting, but the tool needs to be changed from down-milling to reverse milling, which affects the processing quality when fine milling the plane. Therefore, this tool path is usually not used for plane fine milling with high plane quality requirements.
According to the tool path principle determined above, the above workpiece situation can be analyzed. Unidirectional multiple cutting can be used to complete the milling of the same height plane in two times, and the distance between the tool center and the side of the workpiece each time is 20mm.
Specific Processing of the Workpiece
Evenly pad the equal height pads to allow the workpiece to fully contact the equal height pads, and clamp the workpiece with flat-nose pliers. Select a 60mm diameter four-piece small density machine face milling cutter, the spindle forward speed is between 1200~1500; roughly align the Z axis and X axis. Use unidirectional multiple cutting. Each Z axis cut is no more than 0.5mm. Each knife spacing is less than 45mm. The feed speed is controlled between F200~260. After the first milling of the plane, the spindle stops, and the total height of the workpiece is measured perpendicular to the height pad with a depth gauge, and the remaining machining allowance is calculated (there may be a gap of less than 2 wires between the height pad and the workpiece.
If the Z value accuracy requirement is high, do not ignore it). After the calculation is completed, continue to use the same method for processing. Do not directly pierce the surface of the workpiece, and cut away from the workpiece. Finally, leave a finishing allowance of less than 0.3mm, set the spindle high speed finishing, and the speed is not less than 1800, so as to ensure a good surface roughness. During the processing, pay attention to the use of coolant, and sufficient cooling is essential in the entire processing process.
Adjustment of Cutting Parameters
The cutting parameters are restricted by factors such as processing materials, tools, machine tool rigidity, processing routes, and positions, and should be adjusted according to the actual working conditions. The feed rate is adjusted by the manual feed rate switch, and the optimal state is gradually achieved from low to high. If there is a harsh sound or continuous impact sound during processing, it means that the processing parameters are not suitable and should be adjusted in time.
