【Abstract】Before CNC programming, plastic part structure and mold structure should be analyzed first, then entity of heater movable model core should be analyzed to distinguish clearly parting surface, glue plane, ejector hole, inclined top hole, insert, etc. on entity. Block or delete features such as thimble holes, inclined top holes, and stud inserts on core of movable model that do not require CNC machining. Then program surfaces with different functions on moving model core separately, leave a proper margin for collision surface, process glue surface in place, and overcut avoiding surface properly, using tool path milling flow of shape milling road. In order to reflect streamlined structure of curved surface on plastic part, curved surfaces of different structures are programmed separately. Using UG software as a programming tool, CNC milling programming is performed on heater movable model core, programming tool path is simulated.

Machining centers are widely used in processing of mold parts, and most mold parts are processed by machining centers. However, structure of plastic mold parts is very complicated, its surface can be divided into various types of curved surfaces, such as glue level surface, parting surface, bumping surface, etc., can also be divided into various features, such as ejector hole, insert, and inclined top hole, etc. For these features and surfaces on the solid, there are different processing requirements. For the part of glue position on workpiece, it should be finished according to technical requirements; because parting surface on part is used for sealing glue, a proper margin should be left during processing so that operator can assemble mold; when processing void on part, it should be properly over-cut, mainly to facilitate operator to assemble mold; for some special hole positions on part, such as ejector hole, inclined top hole, insert position, etc., these positions do not need to be processed by machining center, but processed by wire cutting or other equipment. In order to prevent these positions from being processed, these features should be deleted or blocked on solid drawing before programming; for corners that cannot be processed, in order to facilitate EDM, a proper margin should be left. Now take movable model core of heater shell as an example to introduce basic steps and methods of CNC programming in detail.

On entity of movable model core, there are several round holes with a diameter of ϕ 6mm. These round holes are mandrel holes, which do not need processing by a machining center and should be deleted from entity; there are 4 studs on plastic part, corresponding position on core is a round hole with a slope, diameter of small head is ϕ 10mm, 4 positions on core are processed by wire cutting and then processed by EDM. They do not need machining center and should be deleted from entity; there are 4 cylinders with a diameter of ϕ 4mm and a height of 6mm on workpiece. These 4 cylinders are inserts on core, which do not need machining center processing and should be deleted from the entity; there are 6 ribs on core, with a width of 1.6mm and a depth of 27mm. These 6 ribs are processed by EDM and need not be processed by a machining center. They should be deleted from entity; There are also runners, water-carrying holes, inclined top positions, etc. on workpiece, which do not need to be processed by machining center and should be deleted from entity. Operation method on UG is to select “Menu→Insert→Synchronous Modeling→Delete Surface” command in order to delete holes, inserts, ribs, runners, etc. on entity. Draw 3 straight lines at the center position to program runner and gate. Core entity is shown in Figure 1.

 

Figure 1 Moving model core entity
a — before entity is arranged b — after entity is arranged

Working environment of machining center in mold factory is very harsh. Affected by jitter of machine tool, wear of machine tool and accuracy of machine tool itself, size of processed workpiece will have errors. If there is an over-cut at sealing position, plastic part will appear flared during injection molding; if assembly position of mold is not processed in place, leaving a margin, it will be difficult to assemble. In order to avoid above two situations, precautions should be taken in advance, a proper margin should be left for sealing position, and position that can be avoided should be appropriately over-cut. In order to make it easier for CNC programmers to write program, it is generally to modify bumping and avoiding positions of entities before programming. On this entity, platform in the middle of upper surface of work piece is bumping position, leaving a margin of 0.02mm, processing method is to lift plane up by 0.02mm; upper surface of locking position is a vacant position, which can be overcut by 0.5mm, processing method is to lower plane by 0.5mm; side of locking position is matching position of fixed mold and movable mold, leaving a margin of 0.02mm, processing method is to offset side by 0.02mm; on parting surface, range within 30mm from glue position does not leave a margin and does not cut, range beyond 30mm from glue position is overcut by 0.5mm, and processing method is to lower plane by 0.5mm. Operation method on UG is to select "Menu→Insert→Design Feature→Extrude" command, use plane that needs to be raised or lowered as sketch plane. If plane needs to be raised, select summation, if plane needs to be lowered, select difference, as shown in picture 2.

 

Figure 2 Editing collision and avoiding positions

Material used is 738 pre-hardened steel with a hardness of 29-33HRC. In order to make surface roughness of processed workpiece meet technical requirements, a tool with higher hardness and better wear resistance should be selected. At present, there are mainly two kinds of tools that meet requirements: one is high-speed tool steel, which is coated with a layer of wear-resistant and oxidation-resistant material on its outer surface to become a tungsten steel knife. Its hardness, wear resistance and heat resistance are high. Normal temperature hardness is generally 89～93HRA, allowable cutting temperature is as high as 800℃～1,000℃, and its hardness remains at 77～85HRA even at 540℃. The other is alloy knife (that is, knife grain knife), which is made of metal carbide, tungsten carbide, titanium carbide, and cobalt-based metal binder through a powder metallurgical process. Its main features are high temperature resistance and high machinability. It can still maintain good cutting performance at around 800-1,000℃, and its cutting speed is 4-8 times higher than that of high-speed steel. High hardness at room temperature and good wear resistance. Bending strength is low, impact toughness is poor, and blade is not easy to sharpen.
In rough machining, due to large cutting amount, alloy cutters (such as ϕ 35R6) should be used for machining. After rough machining, surface allowance of workpiece is uneven, cutting amount in some positions is large, which has a greater impact on tool. It is suitable to use alloy cutters (such as ϕ 17R0.4) for semi-finishing; after semi-finishing, surface allowance of workpiece is basically uniform. For different positions on workpiece, different tools are used for finishing, such as φ 10R5 tungsten steel ball nose tool for curved surface of workpiece; parting surface is flat, which is suitable for φ 17R0.4 alloy cutters; Because distance between pit on upper surface of entity and side of boss is small, this position is processed with a ϕ 10 tungsten steel end mill; runner on core is processed with a ϕ 6R3 tungsten steel ball nose knife, and gate is processed with a tungsten steel ball-end knife of ϕ 4R2.
Since positions of overcutting and overcutting have been sorted out physically, there is no need to overcut or overcut for tool path when performing finishing CNC programming, just set margin to 0. When roughing, choose a cavity milling toolpath with a margin of 0.5mm on one side; for semi-finishing, use a contour milling toolpath with a margin of 0.15mm on one side; for finishing, if it is a curved surface on processing entity, use parallel toolpath, if it is a inclined surface on entity, select contour milling toolpath, if it is plane on processing entity, select plane toolpath, leaving no margin ; If it is a runner on core, use contour tool path.

(1) Select "application module→processing" button in turn, select "cam_general" and "mill_planar" commands in [processing environment] dialog box, click "OK" command to enter UG processing mode.
(2) Click "Geometric View" command button in toolbar, then click "+" in front of "+MCS_MILL" in "Process Navigator-Geometry", select "WORKPIECE" command in the lower commands of "+ MCS_MILL", select "Specify Part" command button in pop-up [Workpiece] dialog box, then select entity; select "Specify Blank" command button, select "Enclosure Block" option in "Type" column in pop-up [Blank Geometry] dialog box, select default parameters in "Limits" column, and click "OK" to set geometry of CNC programming.
(3) Select "Create Tool" button in toolbar to create 6 kinds of tools such as ϕ 35R6 (alloy knife), ϕ 17R0.4 (alloy knife), ϕ 10 (tungsten steel end mill), ϕ 12R6 (tungsten steel ball nose knife) , Φ 6R3 (tungsten steel ball nose knife), ϕ 4R2 (tungsten steel ball nose knife).

In UG, there are many kinds of toolpaths for roughing. Here, "milling with boundary surface" toolpath is used to program roughing toolpath. Specific steps are:
(1) Select "Create Process" command in toolbar, and in pop-up [Create Process] dialog box, select "mill_planar" in "Type" column, select "Face Milling with Boundary" option in "Process Subtype" column, set "Program" to "NC_PROGRAM", "Tool" to "ϕ 35R6", "Geometry" to "WORKPIECE", and "Method" to "METHOD".
(2) Click "OK" button, select "Specify Surface Boundary" button in [Face Milling] dialog box, select 4 edges of parting plane, then set "Cutting Mode" to "Reciprocating", "Step" to "% Tool Straight", "Flat Diameter Percentage" to 65%, “Rough Distance” to 43mm, “Cutting Depth per Cut” to 1mm, and “Final Bottom Surface Allowance” to 0.3mm.
(3) Select "cutting parameters" command button, select "strategy" tab in [cutting parameters] dialog box, set "cutting direction" to "climb milling", "cutting angle" to "designated", "angle with XC" to 180; select "Margin" tab, set "Part margin" to 0.3 mm, "Wall margin" to 0.25mm.
(4) There are several corners on workpiece that need to be processed. When processing corners, tool has a large force-receiving area and cutting edge is easily damaged. Therefore, sharp corner toolpath at the corner should be set as a fillet toolpath. Tool path can be rounded on UG during programming. Steps are as follows: select "corner" tab in [cutting parameters] dialog box, set "lobe" to "roll around object", select "all toolpaths" in "smooth" column, and set "radius" to 50% .
(5) Select "Non-cutting movement" command button, select "Infeed" tab in [Non-cutting movement] dialog box, set "Infeed type" to "Spiral" in "Closed area" column, Diameter" to 10mm, "Ramp angle" to 2°, "height" to 2mm, and "minimum safety distance" to 10mm. In "Open Area" column, set "Infeed Type" to "Linear", "Length" to 10mm, "Height" to 2mm, and "Minimum Safety Distance" to 10mm.
(6) Select "Feedrate and Speed" command button, set "Spindle Speed" to 1,500r/min and "Feedrate" to 2,000mm/min.
(7) Click "Generate" button to generate rough toolpath, as shown in Figure 3.

There are many corners on workpiece. After roughing, corner area has a large margin. A tool path should be designed for corner position to cut corner position margin. Specific step is to first draw 4 rectangular sketches to enclose corner area, use alloy tool of ϕ 17R0.4, use remaining milling tool path in UG to program, and cut uncut corner area of rough tool path. Specific steps are: select "Create Process" command in toolbar, in pop-up [Create Process] dialog box, select "mill_contour" in "Type" column, select "Remaining Milling Contour" in "Process Subtype" column. "" option, set "Program" to "NC_PROGRAM", "Tool" to "ϕ 17R0.4", "Geometry" to "WORKPIECE", and "Method" to "METHOD". Select 4 rectangular sketches as trimming boundary, trim toolpaths other than rectangular sketches, refer to setting method of rough toolpath for setting of other parameters. Toolpath for corner area is shown in Figure 4.

 

Figure 3 Open rough toolpath 

 

Figure 4 Tool path in corner area

After milling of corner area is completed, rough machining is basically completed. At this time, there is a large margin on workpiece, and semi-finishing is required before finishing. Semi-finished tool path uses ϕ 17R0.4 alloy tool, which is processed by contour cutting process. Specific steps are: select "Create Process" command in toolbar, in pop-up [Create Process] dialog box, select "mill_contour" in "Type" column, and select "Depth Contour" in "Process Subtype" column "Milling" option, set "Program" to "NC_PROGRAM", "Tool" to ϕ 17R0.4, "Geometry" to "WORKPIECE", "Method" to "METHOD", select bottom surface as trimming boundary, trim toolpaths other than workpiece, follow setting method of rough toolpath for the rest of parameters. Contour cutting toolpath is shown in Figure 5. When ϕ 17R0.4 alloy knife is processed, distance between rectangular boss on workpiece and side wall of pit is less than diameter of ϕ 17R0.4 alloy knife, cannot be cut; 4 round corners of pit are R7. 5mm, smaller than radius of ϕ 17R0.4 tool, 4 rounded sidewalls are not cut in place, and there is a large margin. In order to cut margin here, use ϕ 10 end mill for cutting, and use remaining milling tool path in UG to program above position. Refer to steps in Figure 4 for specific steps, and tool path is shown in Figure 6.

 

Figure 5 Contour cutting toolpath

 

Figure 6 Cutting margin between rectangular boss and side wall of pit

On moving model core, there are surfaces with different functions such as parting surface, bumping position, glue level surface, avoiding space, locking position, etc., and runner needs to be processed. These surfaces play different roles in moving model core and shape of surface is different. Therefore, when programming toolpaths of these curved surfaces, it is best to write programs separately.
(1) Write finishing program of glue plane. When compiling finishing program of glue plane, processing is carried out according to size of entity, there is no need to leave a margin, and there is no need to overcut. In order to reflect different curved surfaces on workpiece and ensure streamlined corners of workpiece, different tool paths are designed for different structural curved surfaces. There are oblique curved surfaces, rounded curved surfaces, circular arc surfaces, etc. on workpiece. For circular arc curved surfaces, use ϕ 10R5 tungsten steel knife to process parallel cutting toolpaths. For oblique curved surfaces, use ϕ 17R0.4 alloy cutters to cut with contour milling toolpaths. For rounded surface on workpiece, use φ6R3 tungsten steel cutters to process linear toolpaths, as shown in figure Shown in 7a. After machining with a ϕ 6R3 tungsten steel knife with a streamlined tool path, clean root with a ϕ 17R0.4 alloy knife, as shown in Figure 7b. Choosing different tool paths for different curved surfaces best reflects curved surface structure on workpiece.
(2) Program parting surface and void avoidance tool path on parting surface. Parting surface on core and gap avoidance position on parting surface are flat. It is suitable to use alloy knife of ϕ 17R0.4. Since parting surface has already been made to avoid gaps physically, there is no need to avoid gaps again during programming. When parting surface is processed, it should be processed in a solid body, and no allowance is required. Since parting surface is a flat surface, parting surface of core and avoiding gap should be processed with tool path of processing plane. Tool path is shown in Figure 8.

 

Figure 7 Cut different curved surfaces with different toolpaths
a — Cut different surfaces with different toolpaths b — Clear root

 

Figure 8 Design parting surface and toolpath for avoiding gaps on parting surface
a — Tool path for processing parting surface b — Tool path for processing void avoidance
(3) Program tool path of lock position. There are 4 protrusions on 4 corners of parting surface. Its function is to position, prevent core and cavity from being misaligned, to prevent over-cutting due to accuracy of machine tool itself, and to facilitate fitter assembly. When writing program, a margin of 0.03mm is reserved on four raised sides. These 4 raised toolpaths are cut with same height of ϕ17R0.4 alloy knife. Top surface of locking position on entity has been lowered by 0.5mm, and there is no need to overcut top surface by 0.5mm during CNC programming. Specific tool path is a plane milling tool path, which is processed with an alloy cutter of ϕ 17R0.4. Tool path of milling lock position is shown in Figure 9.
(4) Program tool path of boss. There is a rectangular pit (204*54*13mm) on upper surface of core, four corners of pit are rounded R7mm, and there is a boss (125*25*4mm) in the middle of pit. Width between side of boss and side wall of pit is 14.4mm, space between side of boss and side wall of pit cannot be processed with alloy knife of ϕ 17R0.4, but ϕ 10R0 tungsten steel end mills can be used to machine pits and bosses. Plane at the bottom of pit and upper surface of boss are processed by plane milling, side surface and 4 fillets of pit are milled with contour milling toolpaths, as shown in Figure 10.

 

Figure 9 Tool path for designing locking position

 

Figure 10 Design of pit and boss toolpath
(5) Programming runner and pouring position toolpath.
Programming method of processing program of runner and gate is relatively simple. First draw trajectory curve of runner in the center of runner, then use this curved surface to pull out a piece, use tool path driven by curved surface, and runner can be directly processed with forming knife. If gate is a straight gate, you can also use method to process gate, which is very convenient.

After programming of CNC milling machine is completed, in order to check whether tool path is correct and overcut, programmed tool path should be simulated. If tool path is abnormal, abnormal CNC program should be modified. Simulation effect diagram is shown in Figure 11.

 

Figure 11 Simulation effect diagram

Before writing a numerical control program for cavity and core of plastic mold, structure of plastic part and mold structure should be analyzed first, then cavity and core should be analyzed in detail. Different surfaces of part surface (such as glue level surface and contact surface) should be strictly distinguished, features that do not need to be processed on entity should be deleted. Positions on the part that need to be processed by size, positions that need to be avoided, positions that need to leave margins, and positions that need to use electric spark discharge must be fully understood and cannot be confused.
An excellent mold parts CNC programmer, in addition to mastering at least one CNC programming software, must also have a good understanding of processing characteristics of mold parts materials, various structures of mold, characteristics and performance of CNC tools, power and processing range of machining center, in addition, must have long-term practical work experience Before CNC programming, CNC programmers must analyze structure of mold parts, and if necessary, they need to communicate fully with mold designers and mold fitters to understand technical requirements of mold parts in order to write qualified CNC programs. For technicians who have just learned CNC programming, in addition to learning application of programming software, they must also learn basic operations of CNC machine tools, mold structure and material processing characteristics. Only by studying hard can you become an excellent CNC programmer.