德语
Cutting is the main processing method of die parts. However, reasonable process analysis is carried out to correctly calculate the design wire trajectory of the electrode wire in CNC programming, which is related to the processing accuracy of the mold. Improve the cutting process through the determination of threaded holes and the optimization of cutting routes, which is an effective and important way to improve cutting quality and production efficiency.
Calculation of actual trajectory
According to a large number of statistical data, most of the actual size after wire cutting is near the median value (or "middle size") of the tolerance band. Therefore, for the dimensions marked with tolerance in the die part drawing, 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 pattern size outer circle radius R25–0.04, where the bit value dimension is 25+ (0–0.04)/2=24.98 (mm).
Due to the characteristics of wire cutting and discharge processing, there is always a discharge gap between the workpiece and the electrode wire. Therefore, during cutting and processing, the theoretical profile (pattern) of the workpiece should be kept at a certain distance from the actual trajectory of the electrode wire, that is, the vertical distance between the central trajectory of the electrode wire and the outline of the workpiece, which is called the offset f0 (or the compensation value).
f0=R wire + δ electric
Where R wire-electrode wire radius
δ--Single-Side Discharge Gap
For the convex and concave dies of wire cutting processing dies, the electrode wire radius R wire, the single-side discharge gap δ electric, and the single-sided coordination gap δ between the convex and concave dies should be comprehensively considered to determine a reasonable gap compensation value f0.
For example: machining punching die (that is, it is required to ensure the punching size of the workpiece), and the punching punch is referenced, so the gap compensation value of the punch is: f convex = R wire + δ electric, and the size of the concave die should be increased. For processing blanking dies (that is, the workpiece size required to be guaranteed) is based on the blanking die, the gap compensation value of the mold is f convex = R wire + δ electric, and the size of the mold should be increased by δ. See Figure 1.
The magnitude of the offset will directly affect the processing accuracy and surface quality of the wire cutting. If the offset is too large, the gap will be too large and the discharge will be unstable, which will affect the dimensional accuracy; if the offset is too small, the gap will be too small, which will affect the repair and cutting margin. The electrical parameters during repair and cutting will be weakened in turn, and the non-electrical parameters should also be adjusted accordingly to improve the processing quality.
a) Punch (b) Concave Die
According to practical experience, the fitting gap of wire cutting processing punching molds should be smaller than the popular "large" gap punching dies (recommended value of the Manual).
Because during the cutting of convex and concave dies, a melting layer with brittle tissue will form on the surface of the workpiece. The larger the electrical parameters, the worse the surface roughness, and the thicker the melting layer. And as the number of times of punching the mold increases, this brittle surface layer will gradually wear out, causing the fitting gap of the mold to gradually increase, meeting the requirements of "large" gap.
Determination of threaded holes
The position of the threaded hole is very related to the processing accuracy and cutting speed. Generally, the position of the threaded hole is preferably selected at the intersection of known track sizes or at coordinate points that are easy to calculate, so as to simplify the calculation of coordinate sizes in programming and reduce errors.
When cutting a die workpiece with closed-type holes, the threading hole should be located in the center of the model holes, which can not only accurately process the threading holes, but also easily control the calculation of the coordinate trajectory, but the useless cutting stroke is longer. For large hole cutting, the threaded hole can be located near the corners of the processing track to shorten useless stroke.
When cutting the shape of the punch, the thread hole should be selected outside the profile, preferably near the cutting start point. When cutting narrow grooves, the threaded hole should be located at the widest point of the figure, and the threaded hole and the cutting track are not allowed to intersect.
In addition, when more than two workpieces are cut from the same blank, independent thread holes should be installed, and only one thread hole should be installed to cut all workpieces at once. When cutting large punches, those who have the conditions can set up several threading holes along the processing track so that when a wire break occurs during cutting, they can be re-threaded nearby and continue cutting.
The diameter of the threaded hole should be appropriate, generally Φ2mm~Φ8mm. If the hole diameter is too small, it will not only increase the difficulty of drilling but also inconvenient threading; if the hole diameter is too large, it will increase the workload of the fitter. If the number of holes required to be cut is large, the aperture is too small, and the arrangement is dense, smaller thread holes (Φ0.3mm~Φ0.5mm) should be used to avoid the phenomenon of each thread hole being opened to each other or interfering.
Optimization of cutting routes
The rationality of the cutting route will be related to the size of the deformation of the workpiece. Therefore, optimizing the cutting route is conducive to improving cutting quality and shortening processing time. The arrangement of the cutting route should help the workpiece to always keep in the same coordinate system as the clamping support frame during processing, avoid the influence of stress deformation, and follow the following principles.
(1) Under normal circumstances, it is best to arrange the cutting starting point close to 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 close to the clamping end of the blank.
(2) The starting point of the cutting route should be selected where the surface of the workpiece is relatively flat and has less impact on the work performance. For workpieces with high precision requirements, it is best to set the cutting starting point in the prefabricated threading hole on the blank. Do not cut directly from the outside of the blank to avoid deformation of the cut part of the workpiece.
(3) In order to reduce the deformation of the workpiece, 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, we should focus on the optimization of cutting routes.
(1) Secondary (or multiple) cutting method. For some concave model cavity parts with complex shapes, large changes in wall thickness or cross-section, in order to reduce deformation and ensure processing accuracy, the secondary cutting method should be used. Usually, parts with high precision requirements are left with a 2mm~3mm margin for rough cutting first, and after the workpiece has released more deformation, fine cutting is performed to the required size.
In order to further improve the cutting accuracy, before fine cutting, leave a margin of 0.20mm~0.30mm for semi-fine cutting, which is a three-step cutting method. The first time is rough cutting, the second time is semi-fine cutting, and the third time is fine cutting. This is an effective method to improve the accuracy of mold wire cutting processing.
Sharp corner cutting method 2
(3) During the corner secant wire cutting EDM process, the actual position of the electrode wire lags behind the X and Y coordinate axis movement positions of the machine tool due to the reaction force of the discharge, resulting in poor corner accuracy.
The lagging movement of the electrode wire will cause excessive machining of the outer arc of the workpiece and insufficient machining of the inner arc, resulting in reduced accuracy at the corners of the workpiece. For this reason, for corners with high workpiece precision requirements, the driving speed of the X and Y axes should be automatically slowed down so that the actual moving speed of the electrode wire is synchronized with the X and Y axes. That is, 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 inner fillet radius required by the pattern is smaller than the offset during cutting, it will cause an "undercut" phenomenon at the fillet. For this reason, it should be clear that the minimum rounded corner in the pattern outline must be greater than the offset of the last trimming pass, otherwise an electrode wire with a smaller diameter should be selected.
In the main cutting process and the preliminary cutting process, different fillet radii can be set according to the different offsets in each pass of processing, that is, different fillet radius subroutines are compiled for the same segment of the contour. The fillet radius in the subroutine should be greater than the offset of this cutting pass, so that small fillets can be cut and better fillet cutting quality can be obtained.
Preparation of workpiece before cutting
In order to reduce the deformation of the mold during the cutting process and improve the 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 processed with a pair of orthogonal elevations as a benchmark for positioning, calibration and measurement.
(3) Mold cutting should use closed cutting to reduce cutting temperature and deformation.
(4) The amount of material left around the cutting workpiece should be 1/4 of the thickness of the mold, and generally the edge allowance should not be less than 5mm.
(5) In order to reduce mold deformation, correctly select processing methods and strictly implement heat treatment specifications, it is best to perform two tempering treatments for molds with high precision requirements.
(6) All pin holes and screw holes should be processed and formed before quenching the workpiece.
(7) After the heat treatment of the mold, the oxide scale and impurities should be removed from the wire holes to prevent wire breakage caused by reduction in conductive performance.
(8) Before wire cutting, oxide scale and rust should be removed from the surface of the workpiece and degaussed.
Conclusion
After programming is completed and before formal cutting and processing, the prepared program should be checked and verified to determine its correctness.
The CNC systems of wire cutting machine tools all provide program verification methods. Commonly used methods are:
The drawing inspection method is mainly used to verify whether there are syntax errors in the program and whether it conforms to the pattern machining outline; the empty stroke inspection method can verify the actual processing conditions 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 processing inspection method comprehensively verifies the program and processing trajectory by simulating the dynamic machining reality.
Usually, you can run the entire program once and observe whether the graph "returns to zero".
For some dies with high dimensional accuracy requirements and small fitting gaps between convex and concave dies, you can try cutting with thin sheets first to check the dimensional accuracy and fitting gaps. If any discrepancies are found, the procedures should be corrected in time, and formal cutting can only be done after verification.
After the formal cutting is completed, do not rush to remove the workpiece. You should check whether the starting and ending coordinate points are consistent. If any problems are found, "remedial" measures should be taken in time.
Note: All pictures in the article are reprinted online, and will be deleted if infringed!
(2) Sharp corner cutting method. When the workpiece is required to be cut into a "sharp corner" (or "clear corner"), method 1 can be used to add a small overcutting distance to the original route, such as the A0-A1 section shown in Figure 2, so that the maximum lag point of wire electrode cutting reaches the program point A0, and then advances to the additional point A1 and returns to point A0, and then executes the original program to cut the sharp corner.
You can also use the cutting route of Method 2 shown in Figure 3, and add a section of overcut small square or small triangle route at the sharp corner as an additional procedure, so as to ensure that sharp corners with clear edges are cut.
