According to the parts to be turned as shown in the figure below, the material is No.45 steel, and the Ф85 cylindrical surface is not machined. The procedures that need to be performed on CNC lathes are: cutting Ф 80mm and Ф62mm outer circles; R70mm curved surfaces, taper surfaces, undercuts, threads, and chamfers. Requires analysis of process and process routes, preparation of processing procedures.
Turning parts drawing
1. Analysis of parts processing
(1) Setting the workpiece coordinate system
According to the principle of standard coincidence, the origin of the workpiece coordinate system is set at the intersection of the right end face and the rotary axis of the part, as in the Op point in the figure, and the coordinate position of the tool change point relative to the origin coordinate Op of the workpiece coordinate system is set by the G50 command (200,100 )
(2) Select tool
According to the processing requirements of the parts drawing, the end faces, cylindrical faces, conical faces, arc faces, chamfers and cutting thread relief grooves and threads of the machining parts are required to be machined. A total of three tools are required.
No. 1 knife, outer left-handed knife, tool type: CL-MTGNR-2020/R/1608 ISO30. Installed on No. 1 location.
No. 3 knife, thread turning tool, tool type: TL-LHTR-2020/R/60/1.5 ISO30. Mounted on position 3
No. 5 knife, slotted knife, cutter model: ER-SGTFR-2012/R/3.0-0 IS030. Installed on the 5th position.
(3) Processing plan
Use No. 1 outer-circular left-handed knife to finish-machine the end face of the finished part and the outer surface of each part of the part, and leave 0.5 mm of finisher stock for roughing; use No. 5 cutting knife to cut the thread undercut; then Threads are machined using a No. 3 thread cutter.
(4) Determine the cutting amount
Depth of cut: The depth of cut is set to 3mm for roughing and 0.5mm for finish machining.
Spindle speed: According to the cutting performance of No. 45 steel, the cutting speed is set to 90m/min when machining the end face and the outer surface of each segment; the spindle speed is set to 250r/min when threading the car.
Feed rate: Set the feed rate to 200mm/min for roughing and 50mm/min for finish machining. Set the feed speed to 1.5mm/r when turning threads.
2. Programming and operation
(1) Procedures
(2) Program input CNC system
The program is directly input to the CNC system in the CNC lathe MDI mode, or the program is input into the CNC system of the CNC machine tool through the computer communication interface. Then simulate the cutting process on the CRT screen to verify the correctness of the program.
(3) manual knife operation
The workpiece coordinate system is set by tool setting and the tool nose offset value of each tool is recorded. In the running machining program, the offset number of the tool is called to compensate the tool nose offset value.
(4) Automatic machining operations
Select the automatic operation mode, and then press the cycle start button, the machine tool will automatically process the workpiece according to the programmed machining program.
O0001 program code
N005 G50 X200 Z100 Create workpiece coordinate system
N010 G50 S3000 The maximum spindle speed is limited to 3000r/min
N015 G96 S90 M03 Spindle rotation, constant line speed set to 90m/min
N020 T0101 M06 Select No. 1 outer left-handed knife and No. 1 knife-medium
N025 M08 Coolant On
N030 G00 X86 Z0 Tool positioned quickly to cutting position
N035 G01 X0 F50 end face
N040 G00 Z1 Z exits 1mm
N045 G00 X86 X retracts to 86mm to prepare for outer circular cutting cycle
N050 G71 U3 R1 External cutting roughing cycle, cutting depth 3mm, retracting amount 1mm.
N055 G71 P60 Q125 U0.5 W0.5 F200
External cutting roughing cycle, the starting sequence number is N60, the ending sequence number is N125, and 0.5mm finishing allowance is left in the X and Z directions, and the cutting speed is 200mm/min.
N060 G42 Right nose radius compensation, N60～N125 is the finishing line of outer circle cutting cycle
N065 G00 X43.8
N070 G01 X47.8 Z-1
N075 Z-60
N080 X50
N085 X62 Z-120
N090 Z-135
N095 X78
N100 X80 Z-136
N105 Z-155
N110 G02 Z-215 R70
N115 G01 Z-225
N120 X86
N125 G40 Tool radius compensation canceled
N130 G70 P60 Q125 F50 Cylindrical cutting finishing cycle, cutting speed 50mm/min
N135 G00 X200 Z100 Tool return to tool change point
N140 T0505 M06 S50 Select No. 5 slotting cutter and No. 5 offset, constant line speed is set to 50m/min
N145 G00 X52 Z-60 Fast forward to X52, Z-60, ready to cut groove
N150 G01 X45 cutting thread undercut
N155 G04 X2 Pause at the bottom of the slot for 2 seconds
N160 G01 X52 X direction back to 52mm
N165 G00 X200 Z100 Tool return to tool change point
N170 T0303 M06 Select No. 3 thread turning tool and No. 3 tool compensation
N175 G95 G97 S250 Set the cutting speed dimension and set the constant speed to 250r/min.
N180 G00 X50 Z3 Fast forward to X=50, Z=3, ready to turn thread
N185 G76 P011060 Q0.1 R1 thread cutting cycle
N190 G76 X46.38 Z-58.5 R0 P1.48 Q0.4 F1.5
N200 G00 X200 Z100 T0300 Rewind to tool change point and cancel tool compensation No. 3
N205 M05 Spindle stop
N210 M09 Coolant Off
End of N215 M30 program
example:
As shown in the following figure, the machining contents include outside turning and thread turning. The thread turning should be performed after the outer finisher. The parts are processed by using bar blanks. Due to the large amount of blanks, the outer wheel roughing instructions should be used to remove most of the rough stock before leaving the fine outer car. After the roughing car, 0.2 mm margin (unilateral) is left. . According to the processing requirements of the above components, external rough turning tools, outer fine turning tools, grooving tools and thread turning tools are required. The F 62 cylindrical surface is not machined, and the NC machining program for preparing the parts:
CNC Turning Integrated Programming
O0031
N1 G50 X80.0 Z20.0;
N2 G30 U0 W0;
N3 T0101 M03 M08;
N4 G00 X70.0 Z10.0;
N5 G71 U1.0 R1.0;
N6 G71 P7 Q15 U0.4 W0.2 F0.3 S800;
N7 G00 X40.0 F0.15;
N8 G42 G01 X30.0 Z0.0;
N9 G01 Z-25.0;
N10 X40.0;
N11 Z-40.0;
N12 G02 X50.0 Z-45.0 R5.0;
N13 G03 X60.0 Z-50.0 R5.0;
N14 Z-55.0;
N15 G40;
N16 G30 U0 W0;
N17 G50 S1500;
N18 G96 S200 T0202;
N19 G70 P7 Q15;
N20 G00 X62.0 Z0;
N21 X32.0
N22 G01 X-2.0;
N23 G30 U0 W0;
N24 T0404;
N25 G00 X41.0 Z-25.0;
N26 G01 X20.0 F0.15;
N27 G00 X50.0;
N28 G30 U0 W0;
N29 G97 S1500 T0303;
N30 G00 X32.0 Z3.0;
N31 G92 X29.0 Z-22.5 F0.15;
N32 X28.2;
N33 G30 U30.0 W20.0 M09 M05;
N34 M30;