Typically, mold design specifications are proposed by the process engineer based on the specifications of the molded part. Mold manufacturing usually involves several processes: collecting, analyzing, and digesting original data; drawing mold and assembly drawings; proofreading, reviewing, tracing, sending for printing; making all part drawings; trial molding and mold repair; and organizing and archiving data.
Figure 1
To ensure the rationality and consistency of mold manufacturing processes, optimize processing techniques, and improve mold production speed, each mold factory generally develops its own process standards. This article provides a reference standard, focusing on the automotive manufacturing industry, and lists the processes for some important automotive component molds.
Figure 2
1. Process Engineer Compiling Process Cards
When compiling process cards, the process engineer must clearly indicate the machining allowance, the location of the allowance, the surface roughness requirements, and precautions.
Principles for compiling machining process flow cards: Prioritize equipment with high machining efficiency while ensuring accuracy and quality. Milling machines, CNC machines, and grinding machines are faster than wire cutting and EDM, especially EDM, which is the slowest. Dimensions on the drawings cannot be altered arbitrarily.
Figure 3
Note: All templates have been precision machined; the water tank will be returned to the factory for further processing.
After the mold blank returns to the factory, the fitter's requirements are:
1. Are the reference surfaces of plates A and B flush? Are the reference angles right angles?
2. Is the opening and closing of the guide pillars and guide sleeves smooth?
3. Are the screws and threaded holes of the mold frame standard?
4. Is the lower guide pillar and return pin smooth?
5. Are the templates deformed or have blackened surfaces?
Figure 4
Figure 5
Note: The red surface of plates A and B should be roughened with a 3mm allowance; the remaining surfaces must be machined to the required level.
2. Machining Allowance Principles
1. For workpieces requiring heat treatment, add a 0.25mm grinding allowance to each side of the pre-processed outer dimensions before heat treatment.
2. For mold cores and inserts requiring CNC rough machining, allow a 0.2mm allowance to each side.
3. For workpieces requiring rough milling on a fitter's milling machine, allow a 0.3-0.5mm allowance to each side. For workpieces requiring grinding after wire EDM, allow a 0.05mm allowance to each side for shaped parts and a 0.1mm grinding allowance to each side for rough machining of the outer shape.
4. For CNC finishing and EDM followed by mirror polishing, allow a 0.03mm polishing allowance to each side.
3. Machining Accuracy Requirements
The manufacturing accuracy of the mold dimensions should be within the range of 0.005–0.02 mm; the perpendicularity requirement should be within the range of 0.01–0.02 mm; the coaxiality requirement should be within the range of 0.01–0.03 mm; the parallelism requirement of the upper and lower planes of the parting surface of the moving and fixed molds should be within the range of 0.01–0.03 mm.
After mold closing, the gap between the parting surfaces should be less than the overflow value of the molded plastic. The parallelism requirement of the mating surfaces of other mold plates should be within the range of 0.01–0.02 mm; the fitting accuracy of the fixed parts is generally selected within the range of 0.01–0.02 mm; if the small core has no interlocking requirements or has little impact on the dimensions, a double-sided clearance fit of 0.01–0.02 mm can be used; the fitting accuracy of the sliding parts is generally selected from three types: H7/e6, H7/f7, and H7/g6.
Note: If there are inserts with mounting steps on the mirror surface, the fit should not be too tight. Otherwise, when the insert is knocked back from the front, the tool used for knocking may damage the mirror surface. If it does not affect the product dimensions, a gap of 0.01-0.02mm on both sides can be used.
Figure 6
4. Principles of CNC Electrode Removal
For mold cavity cores, the main appearance electrodes should be removed first, then other main electrodes, and finally local electrodes. The appearance electrodes of the fixed mold should be machined as a whole. For areas that cannot be cleared by CNC, wire cutting should be used to clear the corners to ensure a complete and seamless appearance of the fixed mold. For reinforcing ribs, ribs, and pillars with similar depths in the moving mold, they should be machined together on one electrode whenever possible. Deeper ribs should be made into inserts and should be machined separately on the side of the electrode to prevent carbon buildup during electrical pulses. Avoid wire cutting to clear the corners of the moving mold electrodes after CNC milling. If necessary, the electrodes should be disassembled or wire cutting should be used directly. Ribs and rib positions or pillars in the moving mold with a spacing exceeding 35mm should be machined separately to save copper material. For large electrodes, the roughing EDM edge should have a margin of 0.3mm on one side, and the finishing EDM edge should have a margin of 0.15mm on one side. For general electrodes, the roughing EDM edge should have a margin of 0.2mm on one side, and the finishing EDM edge should have a margin of 0.1mm on one side. For small electrodes, the roughing EDM edge should have a margin of 0.15mm on one side, and the finishing EDM edge should have a margin of 0.07mm on one side.
Figure 7
5. CNC Machining Principles
For mold cores and inserts that require CNC roughing, a margin of 0.2mm should be reserved on one side. For workpieces that require CNC finishing after heat treatment, if the product appearance allows, CNC machining should be prioritized for mold cavities and cores that can be finished to the required depth. If CNC machining is not possible, electrodes should be made using electrical discharge machining (EDM).
Figure 8
6. Machining Process for Moving and Static Mold Cores
1) Material Preparation;
2) Milling: Drill water channels (the deepest part of the water channel plug should be 3-4mm from the horizontal water channel), threading holes, drill and tap screw holes, drill and ream ejector pin holes, mark mold number, reference angle, and clearance for the mounting platform;
3) CNC Machining: Rough machining;
4) Heat Treatment: Specify hardness requirements;
5) Grinding: Grind a hexagonal angle ruler, ensuring the outer shape is accurate to the frame dimensions (if the mold core is a single piece, the outer dimensions should be 0.03mm-0.05mm negative than the drawing dimensions; if the mold core is two pieces, the sum of the outer dimensions of the two pieces should be 0.03mm-0.05mm negative than the drawing dimensions), ⊥0.01, ∥0.01. Parts that can be formed by grinding must be ground;
6) For mold cores requiring CNC precision machining, arrange CNC machining. 7) Fine machining: Engraving is required for cavities containing lettering or mold numbers;
8) Wire EDM: Medium wire machining of insert holes, angled ejector holes, ejector pin holes, nozzle holes, etc.;
9) Electrical discharge machining: Machining according to drawings and pulse instruction sheets;
10) Polishing: Specify the polishing roughness and requirements on the process flow card. Mark the polishing areas on the workpiece with a marker. For workpieces requiring a mirror finish, if the timeframe is insufficient, rough polishing can be performed first, followed by fine polishing after trial molding;
11) Assembly and trial molding.
Figure 9
7. Main Inlay Machining Process
1) Material Preparation: The process engineer determines whether the workpiece is being machined as a single piece or multiple pieces together based on its size and shape. If multiple pieces are being machined together, the process engineer needs to create a machining layout drawing for the workpieces.
2) Milling: The fitter performs machining according to the workpiece drawing or the layout drawing provided by the process engineer. This includes drilling water channels (the deepest point of the water channel plug should be 3-4mm from the horizontal water channel), threading holes, drilling and tapping screw holes, drilling and reaming ejector pin holes, roughing the forming area, numbering the mold, and adjusting the mounting table.
3) CNC Machining: For workpieces requiring CNC rough machining, CNC rough machining will be arranged.
4) Heat Treatment: The hardness requirement will be specified.
5) Grinding: The hexagonal angle ruler will be ground. Parts that can be formed by grinding must be ground into shape.
6) For workpieces requiring CNC precision machining, CNC precision machining will be arranged. If the inlay has lettering or mold numbers, engraving is required. 7) Wire EDM: Machining insert holes, angled ejector holes, ejector pin holes, etc., using a medium wire cutter.
8) Electrical Discharge Machining: Machining according to drawings and pulse instruction sheets.
9) Polishing: Specify the polishing roughness and requirements on the process flow card. Mark the polishing areas on the workpiece with a marker. For workpieces requiring a mirror finish, if the cycle time is insufficient, rough polishing can be performed first, followed by fine polishing after trial molding.
10) Assembly and trial molding.
Figure 10
8. Machining Process for Irregularly Shaped Inserts
Process 1:
1) Wire EDM: Accurately cut the outer dimensions using a medium wire cutter (A/B views), pull the sheet, leave thickness allowance, grind, and roughen the forming area.
2) Grinding: Grind the thickness and angle, and form the insert.
3) Electrical Discharge Machining;
4) Polishing.
Process 2:
1) Wire EDM: Cut the outer shape, insert holes, and ejector pin holes with a medium wire cutter, ensuring accurate dimensions (C-view). Roughing the mounting plate and forming area.
2) Grinding: Grind the height, mounting plate, and angle; forming the shape.
3) Electrical Discharge Machining (EDM);
4) Polishing.
9. Angled Ejector Machining Process
1) Wire EDM: Cut the outer shape with a medium wire cutter, grinding the head to fit the insert surface with allowance, ensuring accurate dimensions, leaving allowance for the thickness of the pull tab, and roughing the I-groove with allowance.
2) Grinding: Grind the thickness and I-groove.
3) Assembly;
4) Pulse machining;
5) Polishing;
6) Milling oil grooves.
10. Machining Process for Slanted Top Seat
1) Material Preparation (Fitter): Allow 1.5mm for height on both sides, 0.5mm for width on both sides, and 5mm for length on both sides for easy clamping during wire EDM;
2) Milling: Drill and tap screw holes;
3) Heat Treatment;
4) Grinding: Grind a six-sided angle gauge, ensuring accurate width;
5) Wire EDM: Ensure accurate I-slot machining, pull the sheet, leave thickness allowance, grind, and ensure height is exactly 1.2mm;
6) Grinding: Grind the external dimensions, fit the ejector plate, and ensure height is exactly 1mm.
Figure 11
11. Machining Process for Press Block
1) Material Preparation;
2) Milling: Drill screw holes, roughen the forming area (allow 0.3-0.5mm allowance on one side, grind);
3) Grinding: Grind a six-sided angle gauge, ensure accurate external dimensions, and form the block.
12. Locking Block Machining Process
1) Material Preparation;
2) Grinding: Grind a six-sided angle ruler to ensure accurate external dimensions;
3) Wire EDM: Fast wire forming;
4) Milling: Drill and tap screw holes.
