Wire cutting is the main processing method for die-casting parts. However, reasonable process analysis and accurate calculation of the electrode wire's cutting trajectory in numerical control programming are crucial for the machining accuracy of the mold. Determining the wire-threading hole and optimizing the cutting route to improve the cutting process is an effective way to enhance cutting quality and production efficiency.

Calculation of the Actual Trajectory

A large amount of statistical data shows that the actual dimensions after wire cutting are mostly near the median value (or "middle dimension") of the tolerance band. Therefore, for dimensions with tolerances marked in the die-casting part drawings, the median value should be used as the programming data for the actual cutting trajectory. The calculation formula is: Median value dimension = Basic dimension + (Upper deviation + Lower deviation) / 2.

For example: The drawing dimension of the outer circle radius is R25-0.04, and its median value dimension is 25 + (0-0.04)/2 = 24.98 (mm).

Due to the characteristics of wire-cut electrical discharge machining, there is always a discharge gap between the workpiece and the electrode wire. Therefore, during cutting, a certain distance should be maintained between the theoretical profile (drawing) of the workpiece and the actual trajectory of the electrode wire. This vertical distance between the electrode wire center trajectory and the workpiece profile is called the offset f0 (or compensation value).

f0 = Rwire + δdischarge

Where Rwire -- Electrode wire radius

δdischarge -- Unilateral discharge gap

When wire-cutting the convex and concave dies of a die-casting mold, the electrode wire radius Rwire, the unilateral discharge gap δdischarge, and the unilateral matching gap δmatch between the convex and concave dies should be comprehensively considered to determine a reasonable gap compensation value f0.

For example: When processing a punching die (i.e., ensuring the punching size of the workpiece), the convex die is used as the reference, so the gap compensation value for the convex die is: fconvex = Rwire + δdischarge, and the concave die dimension should be increased by δmatch. When processing a blanking die (i.e., ensuring the size of the blanked workpiece), the concave die is used as the reference, and the gap compensation value for the concave die is fconcave = Rwire + δdischarge, and the convex die dimension should be increased by δmatch. See Figure 1.

The magnitude of the offset will directly affect the machining accuracy and surface quality of the wire cutting. If the offset is too large, the gap will be too large, the discharge will be unstable, and the dimensional accuracy will be affected. If the offset is too small, the gap will be too small, which will affect the trimming allowance. The electrical parameters during trimming will be weakened in turn, and the non-electrical parameters should also be adjusted accordingly to improve the processing quality.

(a) Convex die (b) Concave die

According to practical experience, the matching gap of wire-cut blanking dies should be smaller than the "large" gap dies commonly used internationally (recommended value in the manual).

Because in the wire-cutting processing of convex and concave dies, a layer of brittle and loose molten layer will be formed on the workpiece surface. The larger the electrical parameters, the worse the surface roughness, and the thicker the molten layer. As the number of die-casting times increases, this brittle surface layer will gradually wear away, causing the die matching gap to gradually increase, meeting the requirements of the "large" gap.

Determination of the Wire-Threading Hole

The position of the wire-threading hole is closely related to the processing accuracy and cutting speed. Usually, the position of the wire-threading hole is best selected at the intersection of known trajectory dimensions or at easily calculable coordinate points to simplify the calculation of coordinate dimensions in programming and reduce errors.

When cutting a concave die workpiece with a closed hole, the wire-threading hole should be located in the center of the shaped hole. This allows for accurate processing of the wire-threading hole and convenient control of the coordinate trajectory calculation, but the useless cutting-in stroke is longer. For large shaped hole cutting, the wire-threading hole can be placed near the corner of the processing trajectory to shorten the useless stroke.

When cutting the outer shape of a convex die, the wire-threading hole should be selected outside the shaped surface, preferably near the cutting starting point. When cutting narrow slots, the wire-threading hole should be placed at the widest part of the graphic, and the wire-threading hole is not allowed to intersect with the cutting trajectory.

In addition, when cutting more than two workpieces on the same blank, each workpiece should have its own independent wire-threading hole. Do not use only one wire-threading hole to cut all workpieces at once. When cutting large convex dies, if conditions permit, several wire-threading holes can be set along the processing trajectory, so that if the wire breaks during cutting, it can be re-threaded nearby and continue cutting.

The diameter of the wire-threading hole should be appropriate, generally Φ2mm~Φ8mm. If the hole diameter is too small, it will increase the difficulty of drilling and make it inconvenient to thread the wire; if the hole diameter is too large, it will increase the workload of the fitter. If a large number of shaped holes need to be cut, and the hole diameter is too small and the arrangement is dense, a smaller wire-threading hole (Φ0.3mm~Φ0.5mm) should be used to avoid the wire-threading holes from penetrating each other or interfering with each other.

Optimization of the Cutting Route

The rationality of the cutting route is related to the magnitude of workpiece deformation. Therefore, optimizing the cutting route helps to improve cutting quality and shorten processing time. The arrangement of the cutting route should facilitate the workpiece to remain in the same coordinate system with the clamping support frame during processing, avoid the influence of stress deformation, and follow the following principles.

(1) In general, it is best to arrange the cutting starting point 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 workpiece clamping end.

(2) The starting point of the cutting route should be selected at a relatively flat part of the workpiece surface that has a relatively small impact on the working performance. For workpieces with high precision requirements, it is best to take the cutting starting point in the pre-made wire-threading hole on the blank, and do not directly cut in from the outside of the blank to avoid deformation at the cut opening of the workpiece.

(3) To reduce workpiece deformation, the cutting route should maintain a certain distance from the blank shape, generally no less than 5mm.

For some specific process requirements in wire cutting, the optimization of the cutting route should be paid attention to.

(1) Secondary (or multiple) cutting method For some concave mold cavity parts with complex shapes, large wall thickness, or large changes in cross-section, in order to reduce deformation and ensure processing accuracy, the secondary cutting method should be used. Usually, the parts with high precision requirements leave a margin of 2mm~3mm for rough cutting first. After the workpiece releases more deformation, fine cutting is performed to the required size.

To further improve cutting accuracy, leave a 0.20mm~0.30mm allowance for semi-precision cutting before precision cutting. This is a three-step cutting method: rough cutting, semi-precision cutting, and precision cutting. This is an effective method for improving the precision of mold wire cutting processing.

(2) Sharp Corner Cutting Method When the workpiece needs to be cut into a "sharp corner" (or "clear corner"), method one can be used. Add a short overcut path to the original path, as shown in the A0-A1 segment in Figure 2, so that the maximum lag point of the wire cutting reaches program point A0, then advances to the additional point A1, returns to point A0, and then executes the original program to cut out the sharp corner.

Alternatively, the cutting route of method two shown in Figure 3 can be used. Add a small square or small triangle overcut path at the sharp corner as an additional program to ensure that a sharp corner with clear edges is cut.

Figure 3 Sharp Corner Cutting Method Two

(3) Corner Cutting Method In the wire-cut electrical discharge machining process, due to the reaction force of the discharge, the actual position of the wire is lagging behind the movement position of the machine tool's X and Y coordinate axes, resulting in poor corner accuracy.

The lagging movement of the wire will cause the outer arc of the workpiece to be over-cut and the inner arc to be under-cut, resulting in reduced accuracy at the corners of the workpiece. Therefore, for corners with high workpiece accuracy requirements, the driving speed of the X and Y axes should be automatically slowed down to synchronize the actual movement speed of the wire with the X and Y axes. In other words, the higher the processing accuracy requirement, the slower the driving speed at the corners should be.

(4) Small Fillet Cutting Method If the inner fillet radius required by the drawing is found to be less than the offset during cutting, a "root cutting" phenomenon will occur at the fillet. Therefore, the minimum fillet in the drawing outline must be larger than the offset of the last finishing cut, otherwise, a thinner wire should be selected.

In the main cutting and initial finishing cutting processes, different inner fillet radii can be set according to the different offsets of each pass. That is, different inner fillet radius subroutines can be created for the same segment of the contour. The inner fillet radius in the subroutine should be larger than the offset of this pass, so that a very small fillet can be cut, and better fillet cutting quality can be obtained.

Workpiece Preparation Before Cutting

To reduce the deformation of the mold during cutting and improve processing quality, the convex and concave mold parts should meet the following requirements before cutting:

(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 planes as the positioning, verification, and measurement datum.

(3) Mold cutting should use closed-loop cutting to reduce cutting temperature and deformation.

(4) The allowance around the workpiece to be cut should be 1/4 of the mold thickness, generally not less than 5mm.

(5) To reduce mold deformation and correctly select the processing method and strictly follow the heat treatment specifications, for molds with high precision requirements, it is best to perform two tempering treatments.

(6) Before quenching, all pinholes and screw holes should be machined.

(7) After heat treatment of the mold, the oxide scale and impurities inside the wire holes should be removed to prevent reduced conductivity and wire breakage.

(8) Before wire cutting, the oxide scale and rust on the workpiece surface should be removed, and demagnetization treatment should be performed.

Conclusion

After programming, before formal cutting processing, the compiled program should be checked and verified to ensure its correctness.

The numerical control system of wire cutting machine tools provides methods for program verification. Common methods include:

The drawing inspection method is mainly used to verify whether there are any errors in the program syntax and whether it conforms to the drawing processing contour; the empty stroke inspection method can check the actual processing situation of the program, check whether there is any collision or interference during processing, and whether the machine tool stroke meets the processing requirements; the dynamic simulation processing inspection method simulates the dynamic processing situation to comprehensively verify the program and processing trajectory route.

Usually, the entire program can be run once to observe whether the graphic "returns to zero".

For some punches with high dimensional accuracy requirements and small clearance between convex and concave molds, thin sheet material can be used for trial cutting to check the dimensional accuracy and clearance. If any non-conforming parts are found, the program should be corrected in time until it is verified to be qualified before formal cutting processing.

After the formal cutting is completed, do not rush to remove the workpiece. Check whether the starting and ending coordinates are consistent. If any problems are found, take "remedial" measures in time.