Chapter 4 Mold Manufacturing 4.1 Machining Methods Modern tooling machines for mold making generally feature multiaxial CNC controls and highly accurate positioning systems. The result is higher accuracy and greater efficiency against rejects. Nowadays, heat-treated workpieces may be finished to final strength, up to 2000 MPa, by milling. Various operations, e.g. cavity sinking by EDM, can by replaced by complete milling operations and the process chain thus shortened Furthermore, the thermal damage to the outer zone that would otherwise result from erosion does not occur. hard milling can be used both with conventional cutting-tool materials, such as hard metals, and with cubic boron nitride(CBn). For lastic injection molds, hard metals or coated hard metals should prove to be optimum cutting-tool materials. Machining frees existing residual stresses which can cause distortion either immediately or during later heat treatment. It is advisable, therefore, to relieve stresses by annealing after roughing. Any occurring distortion can be compensated by ensuing finishing which usually does not generate any further stresses After heat treatment, the machined inserts are finished, ground and polished to obtain a good surface quality, because the surface conditions of a cavity are, in the end, responsible for the surface quality of a plastic part and its ease of release Defects in the surface of the cavity are reproduced to different extends depending on the molding material and processing conditions. Deviations from the ideal geometrical contour of the cavity surface, such as ripples and roughness, which increase the necessary release forces Competition has recently developed between high-speed cutting(HSC)and simultaneous five-axis milling. HSC is characterized by high cutting speeds and high spindle rotation speeds Steel maerials with hardness values of up to 62 HRC can also be machined with contemporary tandard HSC millers. Sometimes, HSC machining can be carried out as a complete machining so that the process steps of electrode manufacturing and eroding can be dispensed with completely In addition, better surface quality is often achieved, and this allows drastic reduction in manual postmachining For the production of injection and die-casting molds, a combination of milling and eroding may also be performed. The amount of milling should be maximized since the machining times are shorter on account of higher removal capability. However, very complex contours, filigree geometries and deep cavities can be produced by subsequent spark-erosive machining. The electrode can, in turn, be made from graphite or copper by HsC When machining the part using the CNC machine tool, first prepare the program, ther berate the CNc machine by using the program 1)First, prepare the program from a part drawing to operate the Cnc machine tool 2) The program is to be read into the CNc system. Then, mount the workpieces and tools
Chapter 4 Mold Manufacturing 4.1 Machining Methods Modern tooling machines for mold making generally feature multiaxial CNC controls and highly accurate positioning systems. The result is higher accuracy and greater efficiency against rejects. Nowadays, heat-treated workpieces may be finished to final strength, up to 2000 MPa, by milling. Various operations, e.g. cavity sinking by EDM, can by replaced by complete milling operations and the process chain thus shortened. Furthermore, the thermal damage to the outer zone that would otherwise result from erosion does not occur. Hard milling can be used both with conventional cutting-tool materials, such as hard metals, and with cubic boron nitride (CBN). For plastic injection molds, hard metals or coated hard metals should prove to be optimum cutting-tool materials. Machining frees existing residual stresses which can cause distortion either immediately or during later heat treatment. It is advisable, therefore, to relieve stresses by annealing after roughing. Any occurring distortion can be compensated by ensuing finishing, which usually does not generate any further stresses. After heat treatment, the machined inserts are finished, ground and polished to obtain a good surface quality, because the surface conditions of a cavity are, in the end, responsible for the surface quality of a plastic part and its ease of release. Defects in the surface of the cavity are reproduced to different extends depending on the molding material and processing conditions. Deviations from the ideal geometrical contour of the cavity surface, such as ripples and roughness, which increase the necessary release forces. Competition has recently developed between high-speed cutting (HSC) and simultaneous five-axis milling. HSC is characterized by high cutting speeds and high spindle rotation speeds. Steel maerials with hardness values of up to 62 HRC can also be machined with contemporary standard HSC millers. Sometimes, HSC machining can be carried out as a complete machining so that the process steps of electrode manufacturing and eroding can be dispensed with completely. In addition, better surface quality is often achieved, and this allows drastic reduction in manual postmachining. For the production of injection and die-casting molds, a combination of milling and eroding may also be performed. The amount of milling should be maximized since the machining times are shorter on account of higher removal capability. However, very complex contours, filigree geometries and deep cavities can be produced by subsequent spark-erosive machining. The electrode can, in turn, be made from graphite or copper by HSC. When machining the part using the CNC machine tool, first prepare the program, then operate the CNC machine by using the program. 1) First, prepare the program from a part drawing to operate the CNC machine tool. 2) The program is to be read into the CNC system. Then, mount the workpieces and tools
on the machine, and operate the tools according to the programming. Finally, execute the machining actually Table 4-1: machining plan form for a part Machining process I Side cutti Rough Semi-finish L 2. Machining tools 3. Machining cond Feedrate [4 Tool Before the actual programming, make the machining plan for how to machine the part shown in Table 4-1 and Fig. 4-1. It includes 1)Determination of workpieces machining range 2)Method of mounting workpieces on the machine tool 3)Machining sequence in every machining process 4)Machining tools and machining Side cutting Face cutting Hole machining Fig 4-1: machining plan for a part Reference posit e Present tool position Workpiece 300 Distance to the zero point of a coor. Table Program Fig. 4-2: reference position Fig 4-3: coordinate system specified by the CNC A CNC machine tool is provided with fixed position. Normally, tool change and programming of absolute zero point as described later are performed at this position. This position is called the reference position as shown in Fig 4-2 The tool can be moved to the reference position in two ways 1)Manual reference postion return 2)A The following two coordinate systems are specified at different locations 1) Coordinate system on part drawing. The coordinate system is written on the part
on the machine, and operate the tools according to the programming. Finally, execute the machining actually. Table 4-1: machining plan form for a part. Machining process 1 2 3 Machining procedure Feed cutting Side cutting Hole machining 1.Machining method： Rough Semi-finish Finish 2.Machining tools 3.Machining conditions Feedrate Cutting depth 4.Tool path Before the actual programming, make the machining plan for how to machine the part as shown in Table 4-1 and Fig. 4-1. It includes: 1) Determination of workpieces machining range. 2) Method of mounting workpieces on the machine tool. 3) Machining sequence in every machining process. 4) Machining tools and machining Fig. 4-1: machining plan for a part. Fig. 4-2: reference position Fig. 4-3: coordinate system specified by the CNC A CNC machine tool is provided with fixed position. Normally, tool change and programming of absolute zero point as described later are performed at this position. This position is called the reference position as shown in Fig 4-2. The tool can be moved to the reference position in two ways: 1) Manual reference postion return. 2) Automatic reference position return. The following two coordinate systems are specified at different locations: 1) Coordinate system on part drawing. The coordinate system is written on the part
drawing. As the program data, the coordinate values on this coordinate system are 2) Coordinate system specified by the CNC. The coordinate system is prepared on the actual machine tool table. This can be achieved by programming the distance from the current position of the tool to the zero point of the coordinate system to be set as The positional relation between these two coordinate systems is determined when a workpieces Fixed distance standard p Fixed distance Workpiece zero point Fig 4-4: methods of setting the two coordinate systems in the same position The tool moves on the coordinate system specified by the CNC in accordance with the command program generated with respect to the coordinate system on the part drawing, and cuts a workpiece into a shape on the dray Therefore, in order to correctly cut the workpiece as specified on the drawing, the two coordinate systems must be set at the same position To set the two coordinate systems at the same position, simple methods shall be used according to workpiece shape, the number of machinings 1) Using a stardard plane and point of the workpiece. Bring the tool center to workpiece standard point, and set the coordinate system specified by CNC at this position as shown in Fig 4-4a) 2) Mounting a workpiece directly against the jig. Meet the tool center to the reference position, and set the coordinate system specified by CNC at this position. Jig shall be mounted on the predetermined point from the reference position as shown in Fig 3) Mounting a workpiece on a pallet, then mounting the workpiece and pallet on the jig Jig and coordinate system shall be specified by the same as(2)as shown in Fig 100,30.0,20.0) Command specifying movement from G91 X40.0Y-300Z-100
drawing. As the program data, the coordinate values on this coordinate system are used. 2) Coordinate system specified by the CNC. The coordinate system is prepared on the actual machine tool table. This can be achieved by programming the distance from the current position of the tool to the zero point of the coordinate system to be set as shown in Fig 4-3. The positional relation between these two coordinate systems is determined when a workpiece is set on the table. a) b) c) Fig 4-4: methods of setting the two coordinate systems in the same position The tool moves on the coordinate system specified by the CNC in accordance with the command program generated with respect to the coordinate system on the part drawing, and cuts a workpiece into a shape on the drawing. Therefore, in order to correctly cut the workpiece as specified on the drawing, the two coordinate systems must be set at the same position. To set the two coordinate systems at the same position, simple methods shall be used according to workpiece shape, the number of machinings. 1) Using a stardard plane and point of the workpiece. Bring the tool center to workpiece standard point, and set the coordinate system specified by CNC at this position as shown in Fig 4-4a). 2) Mounting a workpiece directly against the jig. Meet the tool center to the reference position, and set the coordinate system specified by CNC at this position. Jig shall be mounted on the predetermined point from the reference position as shown in Fig 4-4b). 3) Mounting a workpiece on a pallet, then mounting the workpiece and pallet on the jig. Jig and coordinate system shall be specified by the same as (2) as shown in Fig 4-4c)
a)absolute command b)incremental command Fig 4-5: command for moving the tool Command for moving the tool can be indicated by absolute command or incremental command as shown in Fig 4-5. The tool moves to a point at "the distance from zero point of the system"that is to the position of the coordinate values. Incremental command specifies from the previous tool position to the next tool position The speed of the tool with respect to the workpiece when the workpiece is cut is called the cutting speed. As for the CNC, the cutting speed can be specified by the spindle speed in min For example, when a workpiece should be machined with a tool 100mm in diameter at a cutting speed of 80m/min, the spindle speed is approximately 250 min, which is obtained from N=1000v/T D. Hence the following command is required S250 Tool number ATC magazine Fig 4-6: tool function When drilling, tapping, boring, milling or the like, is performed, it is necessary to select a suitable tool. When a number is assigned to each tool and the number is specified in the program, the corresponding tool is selected. For example, when the tool is stored at location 0l in the AtC magazine, the tool can be selected by specifying TOl. This is called the tool function as shown in When machining is actually started, it is necessary to rotate the spindle, and feed coolant. For this purpose, on-off operations of spindle motor and coolant valve should be controlled. The function of specifying the on-off operations of the components of the machine is called the miscellaneous function. In general, the function is specified by an M code. For example, when M03 is specified, the spindle is rotated clockwise at the specified spindle speed Usually, several tools are used for machining one workpiece. The tools have different tool length. It is very troublesome to change the program in accordance with the tools. Therefore, the length of each tool used should be measured in advance. By setting the difference between the length of the standard tool and the length of each tool in the CNC, machining can be performed without altering the program even when the tool is changed This function is called tool length compensation as shown in Fig 4-7. Fig 4-7: tool length Because a cutter has a radius, the center of the cutter path goes around the workpiece with the cutter radius deviated If radiuses of cutters are stored in the cnc, the tool can be moved by cutter radius apart from the machining part figure. This function is called cutter compensation as
a) absolute command b) incremental command Fig 4-5: command for moving the tool Command for moving the tool can be indicated by absolute command or incremental command as shown in Fig 4-5. The tool moves to a point at “the distance from zero point of the coordinate system” that is to the position of the coordinate values. Incremental command specifies the distance from the previous tool position to the next tool position. The speed of the tool with respect to the workpiece when the workpiece is cut is called the cutting speed. As for the CNC, the cutting speed can be specified by the spindle speed in min-1 unit. For example, when a workpiece should be machined with a tool 100mm in diameter at a cutting speed of 80m/min, the spindle speed is approximately 250 min-1, which is obtained from N=1000v/πD. Hence the following command is required: S250. Fig 4-6: tool function When drilling, tapping, boring, milling or the like, is performed, it is necessary to select a suitable tool. When a number is assigned to each tool and the number is specified in the program, the corresponding tool is selected. For example, when the tool is stored at location 01 in the ATC magazine, the tool can be selected by specifying T01. This is called the tool function as shown in Fig 4-6. When machining is actually started, it is necessary to rotate the spindle, and feed coolant. For this purpose, on-off operations of spindle motor and coolant valve should be controlled. The function of specifying the on-off operations of the components of the machine is called the miscellaneous function. In general, the function is specified by an M code. For example, when M03 is specified, the spindle is rotated clockwise at the specified spindle speed. Usually, several tools are used for machining one workpiece. The tools have different tool length. It is very troublesome to change the program in accordance with the tools. Therefore, the length of each tool used should be measured in advance. By setting the difference between the length of the standard tool and the length of each tool in the CNC, machining can be performed without altering the program even when the tool is changed. This function is called tool length compensation as shown in Fig 4-7. Fig 4-7: tool length compensation Because a cutter has a radius, the center of the cutter path goes around the workpiece with the cutter radius deviated. If radiuses of cutters are stored in the CNC, the tool can be moved by cutter radius apart from the machining part figure. This function is called cutter compensation as
hown in Fig 4-8 Cutter path using cutter compensation art Machined pa Fig 4-8: tool cutter compensation In control programs, a number following address g determines the meaning of the command or the concerned block g code list is shown in Table 4-2. g codes are divided into the following 1)One-shot G code. The G code is effective only in the block in which it is specifed 2)Modal G code. The g code is effective until another G code of the same group is specified Table 4-2 G code list G code Grou Function 01 onin Go1 0 Circular interpolation/Helical interpolation G03 01 Circular interpolation/Helical interpolation 00 Dwell, exac G05.1 00 Al advanced control/Al contour control G07.(G107) Advanced preview control G09 G10 Programmable data input 00 Programmable data input mode cancel G15 17 Polar coordinates command cancel 17 Polar coordinates command G17 02 Yp plance selection G1 8 Kp plance selection G19 02 YpZp plance selection Input in inch G21 06 Input in mm function on G23 Store stroke check function off Reference position return check G28 0 Return to reference position eturn from reference position G30 002, 3and 4 reference position return Skip function G33 G37 G39 010000 i automatic tool length measurement Corner offset circular interpolation G40 Cutter compensation canal/Three dimensional compensation cancel G41 Cutter compensation left/Three dimens
shown in Fig 4-8. Fig 4-8: tool cutter compensation In control programs, a number following address G determines the meaning of the command for the concerned block. G code list is shown in Table 4-2. G codes are divided into the following two types: 1) One-shot G code. The G code is effective only in the block in which it is specifed. 2) Modal G code. The G code is effective until another G code of the same group is specified. Table 4-2: G code list G code Group Function G00 01 Positioning G01 01 Linear interpolation G02 01 Circular interpolation/Helical interpolation CW G03 01 Circular interpolation/Helical interpolation CCW G04 00 Dwell, exact stop G05.1 00 Al advanced control/Al contour control G07.1(G107) 00 Cylindrical interpolation G08 00 Advanced preview control G09 00 Exact stop G10 00 Programmable data input G11 00 Programmable data input mode cancel G15 17 Polar coordinates command cancel G16 17 Polar coordinates command G17 02 XPYP plance selection G18 02 ZPXP plance selection G19 02 YPZP plance selection G20 06 Input in inch G21 06 Input in mm G22 04 Store stroke check function on G23 04 Store stroke check function off G27 00 Reference position return check G28 00 Return to reference position G29 00 Return from reference position G30 00 2nd, 3rd and 4th reference position return G31 00 Skip function G33 01 Thread cutting G37 00 Automatic tool length measurement G39 00 Corner offset circular interpolation G40 00 Cutter compensation cancal/Three dimensional compensation cancel G41 00 Cutter compensation left/Three dimensional compensation
G401(G150 19 direction control cancel mode G41.1(G151) hal direction control left side or G42.1(G152) 19 Normal direction control right side on I ler 08 direction G46 G47 Tool offset double increa 00 Tool offset double descrease 08 Tool length compensation cancel GGGG 149 050 11 Programmable mirror image cance G51.1 22 Programmable mirror image 0 Local coordinate system setting G53 00 Machine coordinate system selection 14 Workpiece coordinte system selection 「G54.1 14 Additional workpiece coordinate system selection G55 Work! oordinte system 2 selection G56 14 Workpiece coordinte system 3 selection G57 coordinte system 4 selection G58 4 Workpiece coordinte system selection G60 m Exact stop mode G62 15 Automatic corner override G63 Tapping mode G64 G65 Macro call G66 Macro modal call Macro modal call cancel G68 16 Coordinate rotation/Three dimensional coordinate conversion G69 6 Coordinate rotation cancel/Three dimensional oordinate conversion cancel 09 Peck drilling cycle G74 G75 01 Plunge grinding cycle(for grinding machine G76 09 Fine boring cycle G77 01 Direct constant-dimension plunge grinding cycle for grinding machine) G78 01 Continuous-feed surface grinding cycle(for grinding terni ed surface grinding cycle ( cancel/External operaton function cancel G81 09 Drilling cycle, spot boring cycle or external 09 Drilling cycle or counter boring cycle G83 09 Peck drilling cycle 0 Tapping cycle G85 09Boring cycle G86 Boring cycle
G42 00 Cutter compensation right G40.1(G150) 19 Normal direction control cancel mode G41.1(G151) 19 Normal direction control left side on G42.1(G152) 19 Normal direction control right side on G43 08 Tool length compensation + direction G44 08 Tool length compensation – direction G45 00 Tool offset increase G46 00 Tool offset decrease G47 00 Tool offset double increase G48 00 Tool offset double descrease G49 08 Tool length compensation cancel G50 11 Scaling cancel G51 11 Scaling G50.1 22 Programmable mirror image cancel G51.1 22 Programmable mirror image G52 00 Local coordinate system setting G53 00 Machine coordinate system selection G54 14 Workpiece coordinte system 1 selection G54.1 14 Additional workpiece coordinate system selection G55 14 Workpiece coordinte system 2 selection G56 14 Workpiece coordinte system 3 selection G57 14 Workpiece coordinte system 4 selection G58 14 Workpiece coordinte system 5 selection G59 14 Workpiece coordinte system 6 selection G60 00/01 Single direction positioning G61 15 Exact stop mode G62 15 Automatic corner override G63 15 Tapping mode G64 15 Cutting mode G65 00 Macro call G66 12 Macro modal call G67 12 Macro modal call cancel G68 16 Coordinate rotation/Three dimensional coordinate conversion G69 16 Coordinate rotation cancel/Three dimensional coordinate conversion cancel G73 09 Peck drilling cycle G74 09 Counter tapping cycle G75 01 Plunge grinding cycle (for grinding machine) G76 09 Fine boring cycle G77 01 Direct constant-dimension plunge grinding cycle (for grinding machine) G78 01 Continuous-feed surface grinding cycle (for grinding machine) G79 01 Intermittent-feed surface grinding cycle (for grinding mchine) G80 09 Canned cycle cancel/External operaton function cancel G81 09 Drilling cycle, spot boring cycle or external operation function G82 09 Drilling cycle or counter boring cycle G83 09 Peck drilling cycle G84 09 Tapping cycle G85 09 Boring cycle G86 09 Boring cycle
87 back boring cycle B G91 Increment comm etting for work coordinate system or clamp at maximum spindle speed 92.1 Workpiece coordinate system prese G94 G97 13 Constant surface speed control cancel G98 10 Return to initial point in canned cycle Return to r point in canned cvcle G160 20 In-feed control function cancel (for grindin G161 n-feed control function( for grind 60R Fig 4-9 tool path The tool path in Fig 4-9 can be programmed as follow: G92x200.0Y40.0Z0 G90G03X140.0Y100.0R60.0F300 G02X1200Y60.0R50.0 G92X200.0Y40.0Z0 90G03X140.0Y100.0l-600F300 GO2X1200Y60.0L-50.0 2)In incremental programming G9lG03X-60.0￥60.0R600F300.; G02X-20.0Y-40.0R500 G9lG03X-600Y60.0l-60.0F300 i02X-20.0Y-40.0l-500
G87 09 Back boring cycle G88 09 Boring cycle G89 03 Boring cycle G90 03 Absolute command G91 00 Increment command G92 00 Setting for work coordinate system or clamp at maximum spindle speed G92.1 00 Workpiece coordinate system preset G94 05 Feed per minute G95 05 Feed per rotation G96 13 Constant surface speed control G97 13 Constant surface speed control cancel G98 10 Return to initial point in canned cycle G99 10 Return to R point in canned cycle G160 20 In-feed control function cancel (for grinding machine ) G161 20 In-feed control function ( for grinding machine ) Fig 4-9: tool path programming sample 1 The tool path in Fig 4-9 can be programmed as follow: 1) In absolute programming G92X200.0Y40.0Z0; G90G03X140.0Y100.0R60.0F300.; G02X120.0Y60.0R50.0; or G92X200.0Y40.0Z0; G90G03X140.0Y100.0I-60.0F300.; G02X120.0Y60.0I-50.0; 2) In incremental programming G91G03X-60.0Y60.0R60.0F300.; G02X-20.0Y-40.0R50.0; or G91G03X-60.0Y60.0I-60.0F300.; G02X-20.0Y-40.0I-50.0;
N12 Y轴 刀具直径 具偏置值:+100 X轴 Fig 4-10: tool path programming sample 2 Fig 4-10 is a program example using tool offset. It can be programmed as follow: NIG9lG46G00X80.0Y500D01; N2G47G01X50.0F120.0, N3Y40.0 N4G48X40.0 N5Y-40.0 N6G45X30.0 N7G46G03X30.0J30.0 N8G45G0lY20.0 N9 G46XO Nl0G46G02X-30.0Y30.0J30.0 Nll G45G01Y0 Nl2G47X-120.0; Nl3G47Y-80.0 Nl4G46G00X80.0Y-50.0;
Fig 4-10: tool path programming sample 2 Fig 4-10 is a program example using tool offset. It can be programmed as follow: N1 G91G46G00X80.0Y50.0D01; N2 G47G01X50.0F120.0; N3 Y40.0; N4 G48X40.0; N5 Y-40.0; N6 G45X30.0; N7 G46G03X30.0J30.0; N8 G45G01Y20.0; N9 G46X0; N10 G46G02X-30.0Y30.0J30.0; N11 G45G01Y0; N12 G47X-120.0; N13 G47Y-80.0; N14 G46G00X80.0Y-50.0;
Reference posrtion #3 150 s 1 to 6 Drilling of a 10r 7 to 10 Drilling of a 20mm diameter 11 to 13 Boring of a 95mm diameter hole(depth 50 mm) 250 Initial level X T3 Fig 4-11: tool path programming sample Fig 4-1l is a program example using tool length offset and canned cycles. Offset value +2000 is set on offset no 11+1900 is set in offset no. 15. and +150.0 is set in offset no 31 NOO1 G92XOY0Z0 Coordinate setting at reference position NO02G90G00Z250.0T1lM6 Tool change No03 G43Z0Hll Initial level tool length offset No04 S30M3 Spindle start No5G99G81X4000RY-350.0 Z-1530R-97.0F120 Positioning, then #l drilling N06Y-550.0 Positioning, then #2 drilling and point r level return NO07G98Y-750.0 Positioning, then #3 drilling and initial level return No08G99X1200.0 Positioning, then #4 drilling and point R level return No09Y-550.0 Positioning, then #5 drilling and point R level return NO10G98Y350.0 Positioning, then #6 drilling and initial level return NOll GO0XOYOM5 Reference, then #6 drilling and initial level return Nol2G49Z250.0T15M6 Tool length offset cancel, tool change No13 G43Z0H15 Initial level. tool length offset NO014S20M3; Spindle start Nol5G99G82X550.0￥-450.0
Fig 4-11: tool path programming sample 3 Fig 4-11 is a program example using tool length offset and cannesd cycles. Offset value +200.0 is set on offset No.11 +190.0 is set in offset No.15, and +150.0 is set in offset No.31. ; N001 G92X0Y0Z0; Coordinate setting at reference position N002 G90G00Z250.0T11M6; Tool change N003 G43Z0H11; Initial level, tool length offset N004 S30M3 Spindle start N005 G99G81X400.0RY-350.0 Z-153.0R-97.0F120 Positioning, then #1 drilling N006 Y-550.0 Positioning, then #2 drilling and point R level return N007 G98Y-750.0; Positioning, then #3 drilling and initial level return N008 G99X1200.0 Positioning, then #4 drilling and point R level return N009 Y-550.0; Positioning, then #5 drilling and point R level return N010 G98Y-350.0 Positioning, then #6 drilling and initial level return N011 G00X0Y0M5; Reference, then #6 drilling and initial level return N012 G49Z250.0T15M6; Tool length offset cancel, tool change N013 G43Z0H15; Initial level, tool length offset N014 S20M3; Spindle start N015 G99G82X550.0Y-450.0
Z-1300R-970P300F70 Positioning, then #7 drilling, point R level return No16G98Y-6500; Positioning, then #8 drilling, initial level return NO17G99X1050.0 Positioning, then #9 drilling, point R level return Nol8G98Y-450.0 Positioning, then #10 drilling, initial level return No19 GO0XOYOM Reference position return, spindle stop NO20G49Z250.0T3lM6 Tool length offset cancel tool change No21 G43Z0H31 Initial level tool length offset No22 SIOM3 Spindle start NO23G85G99X800.0Y350.0 Z-153.0R470F50; Positioning, then #ll drilling, point r level return NO24G91Y-200.0K2; Positioning, then #12, 13 drilling, point R level return No25 G28XOYOM5 Reference position return, spindle stop N026G49Z0 Tool length offset cancel NO27 MO: Program stop On the other hand, so far deep hole drilling(gun drilling) has been used more and more widely in injection molds. This method requires a special machine or a deep hole drilling adaptor to another machine, such as a milling machine. The drill operates in a horizontal plane. There are four essential differences from ordinary drilling or milling machines 1)The stroke of the machine( depth of hole)can be considerably larger 2) The drill is supported very close to the work piece, as with a drill jig 3)The cutting edge of the drill is directly, pressure lubricated 4)The drill works in one pass through solid material. It does not require predrilling There are two types of drills, featuring either internal or external chip removal. The external chip removal method is mostly used and is illustrated in Fig. 4-12 C=8 Fig. 4-12: deep hole drilling in cross section 1. Gun Drill material The tip, at the working end of the drill, is made from a tungsten-carbide alloy, which is much harder and longer lasting than high-speed steel. The head is brazed to a long steel tubing, which is held at its other end in the machine chuck. The tip is about 40 mm long when new, the cutting edge can be reground until the length of the remaining head is not long enough to act as a guide within the hole. The shorter the tip the more the risk of wandering 2. Cutting Edge of the Drill The angles of the cutting lips depend on the material to be cut and are about 300 on the short
Z-130.0R-97.0P300F70; Positioning, then #7 drilling, point R level return N016 G98Y-650.0; Positioning, then #8 drilling, initial level return N017 G99X1050.0; Positioning, then #9 drilling, point R level return N018 G98Y-450.0 Positioning, then #10 drilling, initial level return N019 G00X0Y0M5; Reference position return, spindle stop N020 G49Z250.0T31M6; Tool length offset cancel, tool change N021 G43Z0H31; Initial level, tool length offset N022 S10M3; Spindle start N023 G85G99X800.0Y-350.0 Z-153.0R47.0F50; Positioning, then #11 drilling, point R level return N024 G91Y-200.0K2; Positioning, then #12, 13 drilling, point R level return N025 G28X0Y0M5; Reference position return, spindle stop N026 G49Z0; Tool length offset cancel N027 M0; Program stop On the other hand, so far deep hole drilling (gun drilling) has been used more and more widely in injection molds. This method requires a special machine or a deep hole drilling adaptor to another machine, such as a milling machine. The drill operates in a horizontal plane. There are four essential differences from ordinary drilling or milling machines: 1) The stroke of the machine (depth of hole) can be considerably larger. 2) The drill is supported very close to the work piece, as with a drill jig. 3) The cutting edge of the drill is directly, pressure lubricated. 4) The drill works in one pass through solid material. It does not require predrilling. There are two types of drills, featuring either internal or external chip removal. The external chip removal method is mostly used and is illustrated in Fig. 4-12. Fig. 4-12: deep hole drilling in cross section. 1. Gun Drill Material The tip, at the working end of the drill, is made from a tungsten-carbide alloy, which is much harder and longer lasting than high-speed steel. The head is brazed to a long steel tubing, which is held at its other end in the machine chuck. The tip is about 40 mm long when new; the cutting edge can be reground until the length of the remaining head is not long enough to act as a guide within the hole. The shorter the tip, the more the risk of wandering. 2. Cutting Edge of the Drill The angles of the cutting lips depend on the material to be cut and are about 300 on the short
