Wire cutting is the main processing method for stamping die parts, but conducting reasonable process analysis and correctly calculating the design wire trajectory of electrode wires in CNC programming is related to the machining accuracy of the mold. Improving the cutting process by determining threading holes and optimizing cutting routes is an effective and important way to improve cutting quality and production efficiency.
Calculation of actual trajectory
According to a large amount of statistical data, most of the actual dimensions after wire cutting machining are located near the median value (also known as the "middle size") of the tolerance zone. Therefore, for dimensions marked with tolerances in the drawing of stamping die parts, the median size should be used as the programming data for the actual cutting trajectory. The calculation formula is: median size=basic size+(upper deviation+lower deviation).
For example, the outer circle radius of the pattern size is R25-0.04, and the median size is 25+(0-0.04)/2=24.98 (mm).
Due to the characteristics of wire cutting discharge machining, there is always a discharge gap between the workpiece and the electrode wire. Therefore, during cutting processing, the theoretical contour (pattern) of the workpiece should maintain a certain distance from the actual trajectory of the electrode wire, that is, the vertical distance between the center trajectory of the electrode wire and the contour of the workpiece, known as the offset f0 (or compensation value).
F0=R wire+ δ electric
In the formula, R wire - electrode wire radius
δ Electricity - Unilateral discharge gap
The convex and concave molds for wire cutting processing should comprehensively consider the electrode wire radius R wire and unilateral discharge gap δ Unilateral fit gap between electrical and convex and concave molds δ To determine a reasonable gap compensation value f0.
For example, when machining a punching die (which requires ensuring the punching size of the workpiece), the clearance compensation value of the punch is: f convex=R wire, based on the punching punch as the benchmark+ δ The size of the electric and concave molds should be increased δ Matching. When processing the blanking die (i.e. ensuring the size of the workpiece to be punched), the gap compensation value f convex=R wire of the blanking die is used as the benchmark+ δ The size of the electricity and punch should be increased δ Matching. See Figure 1.
The offset will directly affect the machining accuracy and surface quality of wire cutting. If the offset is too large, the gap is too large, the discharge is unstable, and the dimensional accuracy is affected; If the offset is too small, the gap is too small, which will affect the trimming allowance. The electrical parameters during trimming processing will gradually weaken, and non electrical parameters should also be adjusted accordingly to improve processing quality.
(a) Male mold (b) Female mold
Based on practical experience, the fit clearance of wire cutting punching molds should be smaller than the internationally popular "large" clearance punching molds (recommended in the manual).
Due to the formation of a brittle and loose melting layer on the surface of the workpiece during wire cutting of convex and concave molds, the larger the electrical parameters, the poorer the surface roughness, and the thicker the melting layer. And as the number of times the mold is punched increases, the brittle and loose surface layer will gradually wear out, causing the fit gap of the mold to gradually increase, meeting the requirement of a "large" gap.
Determination of threading holes
The position of the threading hole is closely related to the machining accuracy and cutting speed. Usually, it is best to choose the position of the threading hole at the intersection of known trajectory dimensions or coordinate points that are convenient for calculation, in order to simplify the calculation of coordinate dimensions in programming and reduce errors.
When cutting concave die workpieces with closed holes, the threading hole should be located at the center of the hole, which can accurately process the threading hole and conveniently control the calculation of coordinate trajectory. However, the unnecessary cutting stroke is longer. For large hole cutting, threading holes can be located near the edges and corners of the machining trajectory to shorten unnecessary travel.
When cutting the convex mold shape, the threading hole should be selected outside the mold surface, preferably located near the cutting starting point. When cutting narrow grooves, the threading hole should be located at the widest point of the figure, and it is not allowed to intersect with the cutting trajectory.
In addition, when cutting two or more workpieces on the same blank, separate threading holes should be set up, and not just one threading hole can cut all workpieces at once. When cutting large convex molds, if conditions permit, several threading holes can be set along the machining trajectory, so that when wire breakage occurs during cutting, the wire can be re threaded nearby to continue cutting.
The diameter of the threading hole should be appropriate, usually Φ 2mm~ Φ 8mm。 If the aperture is too small, it increases the difficulty of drilling and is not convenient for threading; If the aperture is too large, it will increase the workload of the fitter. If a large number of cutting holes are required, the aperture is too small, and the arrangement is relatively dense, smaller threading holes should be used（ Φ 0.3mm~ Φ 0.5mm) to avoid mutual penetration or interference between each threading hole.
Optimization of cutting route
The rationality of the cutting route will affect the magnitude of workpiece deformation. Therefore, optimizing the cutting route is beneficial for improving cutting quality and shortening processing time. The arrangement of the cutting route should be conducive to keeping the workpiece in the same coordinate system as the clamping support frame during the machining process, avoiding the influence of stress deformation, and following the following principles.
(1) In general, it is best to arrange the starting point of cutting near the clamping end, arrange the cutting section that separates the workpiece from its clamping part at the end of the cutting route, and set the pause point near the clamping end of the blank.
(2) The starting point of the cutting route should be selected at a location where the workpiece surface is relatively flat and has little impact on the working performance. For workpieces with high precision requirements, it is best to take the cutting starting point in the pre made threading hole on the blank, and not directly cut into it from the outside of the blank to avoid deformation at the cutting point of the workpiece.
(3) To reduce workpiece deformation, a certain distance should be maintained between the cutting route and the shape of the blank, generally not less than 5mm.
For some specific process requirements in wire cutting processing, it is important to focus on optimizing the cutting route.
(1) For some concave cavity parts with complex shapes, wall thickness, or large cross-sectional changes, the secondary (or multiple) cutting method should be used to reduce deformation and ensure machining accuracy. Usually, areas with high precision requirements are left with a margin of 2mm~3mm for rough cutting, and after the workpiece releases more deformation, fine cutting is carried out to the required size.
If, in order to further improve the cutting accuracy, a margin of 0.20mm~0.30mm is left for semi precision cutting before precision cutting, which is a three step cutting method. The first step is rough cutting, the second step is semi precision cutting, and the third step is precision cutting. This is an effective method to improve the accuracy of mold wire cutting machining.
(2) When the sharp angle cutting method requires the workpiece to be cut into a "sharp angle" (also known as "clear angle"), Method 1 can be used by adding a small section of the over cutting path on the original path, as shown in A0-A1 section in Figure 2, so that the maximum lag point of the electrode wire cutting reaches program A0 point, then advances to the additional point A1 and returns to A0 point, and then executes the original program to cut out the sharp angle.
Alternatively, the cutting route of Method 2 as shown in Figure 3 can be used by adding an over cut small square or triangle route at the sharp corners as an additional procedure, which ensures that sharp corners with clear edges can be cut.
Figure 3 Sharp Corner Cutting Method 2
(3) During the process of corner cutting and discharge machining, the actual position of the electrode wire lags behind the X and Y coordinate axes of the machine tool due to the reaction force of the discharge, resulting in poor corner accuracy.
The lagging movement of the electrode wire can cause excessive processing of the outer arc of the workpiece, while insufficient processing of the inner arc leads to a decrease in accuracy at the corners of the workpiece. Therefore, for corners with high precision requirements for the workpiece, the driving speed of the X and Y axes should be automatically slowed down to synchronize the actual movement speed of the electrode wire with the X and Y axes. That is to say, the higher the machining accuracy requirement, the slower the driving speed at the corner should be.
(4) If the small fillet cutting method finds that the required inner fillet radius in the drawing is less than the offset during cutting, it will cause the phenomenon of "undercutting" at the fillet. Therefore, it should be clear that the minimum fillet in the contour of the pattern must be greater than the offset of the last trimming, otherwise a finer diameter electrode wire should be selected.
In the main cutting process and initial cutting process, different inner fillet radii can be set according to the different offsets during each processing, that is, different inner fillet radii subroutines can be developed for the same contour segment. The inner fillet radius in the subroutine should be greater than the offset of this cutting process, which can cut very small fillets and achieve good fillet cutting quality.
Preparation of the workpiece before cutting
In order to reduce mold deformation during the cutting process and improve processing quality, the convex and concave mold parts before cutting should meet the following requirements:
(1) The parallelism error between the upper and lower planes of the workpiece should be less than 0.05mm.
(2) The workpiece should be machined with a pair of orthogonal facades as a reference for positioning, calibration, and measurement.
(3) Mold cutting should adopt closed cutting to reduce cutting temperature and deformation.
(4) The margin of edge material around the cutting workpiece should be 1/4 of the mold thickness, and generally the margin of edge material should not be less than 5mm.
(5) To reduce mold deformation, correctly select processing methods, and strictly follow heat treatment specifications, it is best to perform two tempering treatments for molds with high precision requirements.
(6) Before quenching the workpiece, all pin holes and screw holes should be machined into shape.
(7) After heat treatment of the mold, oxide skin and impurities should be removed from the threading hole to prevent wire breakage caused by reduced conductivity.
(8) Before wire cutting, the surface of the workpiece should be cleaned of oxide skin and rust, and undergo demagnetization treatment.
epilogue
After programming is completed and before formal cutting and processing, the compiled program should be checked and verified to determine its correctness.
The CNC system of wire cutting machine tools provides program verification methods, commonly used methods include:
The drawing verification method is mainly used to verify whether there are errors in syntax and whether it conforms to the contour of the pattern processing in the program; The empty stroke inspection method can verify the actual processing situation of the program, check whether there is collision or interference during processing, and whether the machine tool stroke meets the processing requirements; The dynamic simulation machining inspection method comprehensively verifies the program and machining trajectory path by simulating the actual dynamic machining situation.
Usually, you can run all the programmed programs once and observe whether the graphics are "reset".
For some stamping dies with high dimensional accuracy requirements and small clearance between convex and concave molds, thin sheet materials can be used for trial cutting to check the relevant dimensional accuracy and clearance. If any discrepancies are found, the program should be corrected in a timely manner until it is verified to be qualified before formal cutting and processing can be carried out.
After the formal cutting is completed, the workpiece should not be hastily removed. The starting and ending coordinate points should be checked for consistency. If any problems are found, timely "remedial" measures should be taken.