CNC Machinery Module 4: CNC Programming "Turning" PREPARED BY IAT Curriculum Unit August 2009 Institute of Applied Technology, 2009
2 Module 4: CNC Programming "Turning"
Module 4: CNC Programming "Turning" Module Objectives: 1. Identify the different parts that compose the program. 2. Utilize both preparatory functions (G-codes) and miscellaneous functions (M-codes). 3. Demonstrate the ability to write a program to manufacture a simple workpiece using the MTS simulator. 4. Use some canned cycles in turning supported by the (SINUMERIK 840D) controller. 5. Utilize subprograms programs. 6. Verify the program graphically on the computer. Module Contents Topic Page No. 1 Structure of NC-program 4 2 Preparatory, additional and switching functions 5 3 How to write an NC program 7 4 Practical Tasks 12 Module 4: CNC Programming "Turning" 3
1.. Structure of an NC Program: The NC program consists of a series of commands with which the CNC machine tool is instructed to manufacture a certain work part. Fig. 4.1 1.1 Program beginning: it consists of a character (%) which informs the controller that an NC Program will follow. Everything stands before this character is ignored by the controller. The first line in the NC Program contains the program name. 1.2 Program core: it consists of a sequence of blocks (Lines). Each block contains the technical and geometric information that the controller requires for the correspondent machining step. It starts always with the block Number (N) e.g. N10, then the instructions or commands follow. 1.3 Program end: it consists of one block having one command which is M30. Fig. 4.1 Structure of an NC Program 4 Module 4: CNC Programming "Turning"
2.Preparatory, additional and switching functions: Four groups of instructions can be differentiated: 2.1 G-functions: G functions are codes determine the geometric part of the NC program. Some important G-Codes in the table below: Function G00 G01 G02 G03 G04 G20 G21 G54 G90 G91 G92 G94 G95 G96 G97 Description Rapid positioning; the tool will move to the target point in rapid speed Feed rate positioning; the tool will move to the target point according the feed rate speed Arc clockwise Arc counter clockwise Dwell; the tool will hold in place for a specific amount of time, and then continues; e.g. G04 X5, the tool will wait for 5 seconds. Inch units Metric units Work piece coordinate setting Absolute positioning; the tool will move to the target point according to absolute dimensions. Incremental positioning; the tool will move to the target point according to incremental dimensions. Max. Spindle speed limit. Feed rate (F) in mm/min., mainly for milling Feed rate (F) in mm/rev., mainly for turning Constant Cutting Speed Cancel Constant Cutting Speed Module 4: CNC Programming "Turning" 5
2.2 Coordinates (X, Y & Z): they are used in a block to locate the target point where the tool should go. In turning machines, tools follow 2 axes only, X & Z. 2.3 Additional and switching functions: Function Description F S T M3 M4 M5 M6 M7 M8 M9 M17 M30 TRANS Feed rate Speed Tool position Spindle rotation clockwise Spindle rotation counter clockwise Spindle stop Tool change Flood coolant #1 ON Flood coolant #2 ON Coolant OFF Subprogram end Program end Zero point Shift 6 Module 4: CNC Programming "Turning"
2.4 Cycles: A cycle allows performing a complete machining operation by specifying just one code. Cycle Cycle 81 Cycle 83 Cycle 93 Cycle 95 Cycle 97 Description Drilling; to make a hole in one phase. Deep Drilling (Pecking); to make a deep hole, which requires introducing the tool with several phases.(chip-breaking and chip removal) Recessing; to make an internal or external groove. Canned cycle (roughing and finishing cycle); to cut the material following a pre-set contour using a subprogram. Tapping; to make an internal or external thread. 3. How to write an NC program: The program beginning consists of a character or a command (ex. %) which informs the CNC-control that a NC-program will follow. The first line in the NC program contains the program name (ex. TP0147). The NC-program names can contain alphanumerical (containing letters and numbers) or numerical characters. For most CNC-controls, 2-6 digit character sequences are used for identification. An NC-program consists of order sequence of blocks. They contain the geometric and technical information that the CNC-control requires for each machining step. Everything stands before the character % for commenting the program is ignored by the control. Program end M30 The program end is commanded with M30. Important note Everything that stands before the character % for commenting the program is ignored by the control. Comments are also allowed within the program, these must be set in brackets. Module 4: CNC Programming "Turning" 7
Example 1: Rapid traverse in absolute dimensioning. N30 G90 N40 G00 X30 Z5 The tool will move to the target point with rapid speed, following the absolute dimensioning system is shown in Fig. 4.2. Fig. 4.2: Rapid Traverse in absolute dimensioning. Example 2: Rapid traverse in incremental dimensioning. N70 G91 N80 G00 X-12.5 Z-35 The tool will move to the target point with rapid speed, following the incremental dimensioning system shown in Fig. 4.3. Fig. 4.3: Rapid traverse in incremental dimensioning. 8 Module 4: CNC Programming "Turning"
Example 3: Feed rate traverse in absolute dimensioning. N120 G90 N130 G01 X140 Z-90 The tool will move in linear motion to the target point with feed rate speed, following the absolute dimensioning system as illustrated in Fig. 4.4. Fig. 4.4: Feed rate traverse in absolute dimensioning. Example 4: Feed rate traverse in incremental dimensioning. N50 G91 N60 G01 X20 Z-60 The tool will move in linear motion to the target point with feed rate speed, following the incremental dimensioning system as illustrated in Fig. 4.5. Fig. 4.5: Feed rate traverse in incremental dimensioning. Module 4: CNC Programming "Turning" 9
Arcs clockwise and counter clockwise. When an arc is to be machined, the interpolation parameters I, J & K must be specified. These parameters are used to define the center of a circle for circular movements as explained by Fig. 4.6. Fig. 4.6: I, and K parameters. "I" is the distance between the starting position and the circle center in the X- direction. "J" is the distance between the starting position and the circle center in the Y- direction. "K" is the distance between the starting position and the circle center in the Z- direction. Since in turning there is no Y-axis, then J is always zero and no need to mention it in the block; 10 Module 4: CNC Programming "Turning"
Example 5: Programming using G02 for clockwise Arc. See Fig. 4.7 N50 G01 X80 Z-40 N60 G02 X140 Z-106 I+45 K-20 Fig. 4.7: Programming using G02. Example 6: Programming using G03 for Counterclockwise Arc. Refer to Fig. 4.8 N50 G01 X80 Z-50 N60 G03 X140 Z-80 I-15 K-45 Fig. 4.8: Programming using G03. Module 4: CNC Programming "Turning" 11
Practical Tasks Practical Task (1) Title: Facing Create an NC program making 1 mm facing. The workpiece shown in the drawing below is the finished part. Parameters: o Chuck type: outside. o Chucking depth: 15 mm o Material: Aluminum Almg1 o Zero point: right workpiece side o Tool: Left Corner Tool, CL-SCLCL 2020 L 1208 ISO30 o Max. spindle speed limit: 2000 RPM o Constant cutting speed: 200 m/min o Feed rate: 0.2 mm/rev. o Spindle rotation: counter clockwise 12 Module 4: CNC Programming "Turning"
*Hints: 1-To create an NC program, use the following procedure: a. Setup form (tools) using setup mode; described in module 3. b. Setup sheet using setup dialog; described in module 3. c. Main program using editor. 2-While programming in editor you can always use the function renumber to reorganize the blocks numbers. 3-You can use shift + insert to insert a new line above. Solution: N10 G54 N15 G92 S2000 N20 T1 D1 M6 N25 G96 S200 F0.2 M4 N30 G0 X43 Z0 N35 G1 X-2 N40 G1 Z2 N45 G0 X150 Z150 N50 M30 Module 4: CNC Programming "Turning" 13
Practical Task (2) Title: Turning Using the same tool used in practical task (1), create an NC Program to produce the finished workpiece shown in the drawing below. It is needed to make a 1 mm facing operation prior to parallel turning; all dimensions are in mm. Parameters: o Chuck type: outside. o Chucking depth: 15 mm o Material: Aluminum Almg1 o Zero point: right workpiece side o Tool: Left Corner Tool, CL-SCLCL 2020 L 1208 ISO30 o Max. spindle speed limit: 2000 RPM o Constant cutting speed: 200 m/min. o Feed rate: 0.3 mm/rev. o Spindle rotation: counter clockwise 14 Module 4: CNC Programming "Turning"
*Hint: If the tool is moving along one axis, no need to mention the coordinate on the second axis. Possible solution: N10 G54 N15 G92 S2000 N20 T1 D1 M6 N25 G96 S200 F0.3 M4 N30 G0 X42 Z0 N35 G1 X-2 N40 G1 Z2 N45 G0 X45 Z0 N50 G1 X38 Z0 N55 G1 X38 Z-40 N60 G1 X40 Z-40 N65 G0 X40 Z0 N70 G1 X36 Z0 N75 G1 X36 Z-40 N80 G1 X38 Z-40 N85 G0 X38 Z0 N90 G1 X34 Z0 N95 G1 X34 Z-40 N100 G1 X36 Z-40 N105 G0 X36 Z0 N110 G1 X32 Z0 N115 G1 X32 Z-40 N120 G1 X34 Z-40 N125 G0 X34 Z0 N150 G1 X30 Z0 Module 4: CNC Programming "Turning" 15
N155 G1 X30 Z-40 N240 G1 X31 Z-40 N245 G0 X31 Z0 N250 G0 X150 Z150 N255 M30 Practical Task (3) Title: Turning (using cycle 95) Create an NC Program to produce the finished workpiece shown in the drawing below using cycle 95. It is needed to make a 1 mm facing operation prior to taper turning; all dimensions are in mm. Parameters: o Chuck type: outside. o Chucking depth: 15 mm o Material: Aluminum Almg1 o Zero point: right work part side o Tools: Pos#1: Left Corner Tool, CL-SCLCL 2020 L 1208 Pos#2: Left Corner Tool, CL-SVJCL 2020 L 1604 o Max. spindle speed limit: 2000 RPM o Constant cutting speed: 200 m/min o Feed rate: 0.3 mm/rev o Spindle rotation: counter clockwise 16 Module 4: CNC Programming "Turning"
Possible solution: 1-Subprogram (L1205): Use the editor to write the following subprogram. N20 G1 X40 Z0 N25 G1 X20 Z-40 N25 G1 X40 Z-40 N30 G1 X42 Z-40 N30 M17 Save the subprogram under the name L1205. Module 4: CNC Programming "Turning" 17
2-Main program: N10 G54 N15 G92 S2000 N20 T1 D1 M6 N25 G96 S200 F0.3 M4 N30 G0 X42 Z0 N35 G1 X-2 N40 G1 Z2 N45 G0 X42 Z2 N50 G0 X150 Z150 N55 T2 D1 M6 N60 G0 X42 Z2 N65 CYCLE95 ("L1205",2,0,0,0,0.2,0.1,0.1,1) N70 G0 X150 Z150 N80 M30 18 Module 4: CNC Programming "Turning"
Practical Task (4) Title: Recessing (using Cycle 93) Create an NC Program to produce the finished work part shown in the drawing below. It is needed to make 1 mm facing operation and using cycle 95 for parallel turning. All dimensions are in mm. All chamfers are 1mm x 45. (Use absolute dimensioning). Parameters: o Chuck type: outside. o Chucking depth: 15mm o Material: Aluminum Almg1 o Zero point: right work part side o Tools: Pos#1: Left Corner Tool, CL-SCLCL 2020 L 1208 Pos#2: Recessing Tool, ER-SGTFL 1212 L 1.85 o Max.spindle speed limit: 2000 RPM. o Constant cutting speed: 200 m/min. for parallel turning and 125 for recessing. Module 4: CNC Programming "Turning" 19
o Feed rate: 0.3 mm/rev. for parallel turning and 0.08 mm/rev. for recessing. o Spindle rotation: counter clockwise *Hint: You can use the start-tag / end-tag commands in editor to copy/paste similar programs already done. Possible solution: 1.Subprogram: Use the editor to write the following subprogram. N10 G1 X30 Z1 N15 G1 X30 Z0 N75 G1 X30 Z-60 N80 G1 X42 Z-60 N65 M17 Save the subprogram under the name L89. 2.Main program: N10 G54 N15 G92 S2000 N20 T1 D1 M6 N25 G96 S200 F0.3 M4 N30 G0 X42 Z0 N35 G1 X-2 N40 G1 Z2 N45 G0 X42 Z2 N50 G1 X41 Z2 20 Module 4: CNC Programming "Turning"
CYCLE95 ("L89",2,0.2,0.2,0.2,0.2,0.1,0.1,3) N360 G1 X42 Z-39 N250 G0 X150 Z150 N255 T2 D1 M6 N260 G96 S125 F0.08 M4 N265 G0 X32 Z-10 N270 G1 X30 Z-10 N280 CYCLE93 (30,-10,7.5,2,0,0,0,-1,-1,0,0,0.2,0.3,1.5,1,5) N285 G0 X32 Z-27.5 Module 4: CNC Programming "Turning" 21
N290 G1 X30 Z-27.5 N295 CYCLE93 (30,-27.5,5,5,0,0,0,-1,-1,0,0,0.2,0.3,1.5,1,5) N300 G1 X32 Z-42.5 N305 G1 X30 Z-42.5 N310 CYCLE93 (30,-42.5,7.5,2,0,0,0,-1,-1,0,0,0.2,0.3,1.5,1,5) N315 G0 X150 Z150 N320 M30 22 Module 4: CNC Programming "Turning"
Practical task (5) Title: Threading (using cycle 97) Create an NC Program to produce the finished work part shown in the drawing below. It is needed to make 1 mm facing operation prior to parallel turning. All dimensions are in mm. Parameters: o Chuck type: outside. o Chucking depth: 15mm o Material: Aluminum Almg1 o Zero point: right work part side o Tools: Pos#1: Left Corner Tool, CL-SCLCL 2020 L 1208 Pos#2: Left Threading Tool, TL-LHTR 2020 R 60 2.5 o Max. spindle speed limit: 2000 RPM o Constant cutting speed: 200 m/min. for parallel turning o Spindle Speed for threading: 800 RPM o Feed rate: 0.3 mm/rev. o Spindle rotation: counter clockwise for parallel turning and clockwise for threading Module 4: CNC Programming "Turning" 23
Possible solution: 1-Subprogram (L90): N10 G1 X20 Z2 N15 G1 X20 Z0 N75 G1 X20 Z-40 N80 G1 X40 Z-40 N55 M17 2-Main program: N10 G54 N15 G92 S2000 N20 T1 D1 M6 N25 G96 S200 F0.3 M4 N30 G0 X42 Z0 N35 G1 X-2 N40 G1 Z2 N45 G0 X41 Z2 N50 CYCLE95 ("L90",2,0.2,0.25,0,0.1,0.15,0.1,1) N50 G0 X150 Z150 N250 T2 D1 M6 N255 M5 N260 G97 S800 F0.3 M4 24 Module 4: CNC Programming "Turning"
N265 CYCLE97 (2.5,,0,-35,20,20,10,0,1.25,0.02,29,0,30,4,3,1) Module 4: CNC Programming "Turning" 25
((The following are the tables and information required to fill the parameters of cycle 97)) IANG: 26 Module 4: CNC Programming "Turning"
N270 G1 X70 Z0 N275 G0 X150 Z150 N270 M30 Module 4: CNC Programming "Turning" 27
Practical task (6) Title: CNC Turning Project. Using the MTS Simulation software, create an NC Program in order to manufacture the mechanical shaft shown in the technical drawing below. 1. Technical Drawing Overall diameter = 60mm; All chamfers are 1 x 45 2. Machining Steps a. Facing b. Parallel Turning c. Recessing d. Threading e. Center Drilling f. Drilling 28 Module 4: CNC Programming "Turning"
Hints: It is up to the programmer to choose the suitable setup parameters according to the material and the dimensions of the finished work part. Direction of rotation is related to the tool in use. 3. Programming Steps a-tools Preparation: i.tool in position 1 Left Corner Tool CL-SCLCL 2020 L 1208 ISO30 ii.tool in position 5 Recessing Tool ER-SGTFL 2012 L 02.00-0 ISO30 iii.tool in position 6 Left Threading Tool TL-LHTR 2020 R 60 3.5 ISO30 iv.tool in position 7 Spotting Drill DR-15.00 034 L HSS ISO30 Module 4: CNC Programming "Turning" 29
v.tool in position 9 Twist Drill DR-15.00 067 L HSS ISO30 b- Subprogram (L150): N10 G1 X26 Z2 N15 G1 X30 Z-1 N20 G1 X30 Z-20 N25 G1 X33 Z-20 N30 G1 X35 Z-21 N35 G1 X35 Z-30 N40 G1 X38 Z-30 N45 G1 X40 Z-31 N50 G1 X40 Z-60 N55 G1 X41 Z-60 N60 G3 X45 Z-62 I0 K-2 N65 G1 X45 Z-70 N70 G1 X60 Z-100 N75 G1 X60 Z-110 N80 G1 X65 Z-110 N85 M17 30 Module 4: CNC Programming "Turning"
C- Main Programming i- Machine Setup: in order to set the machine, a setup sheet is created, where all the following has to be mentioned: 1. Chucking device 2. Chuck s dimensions 3. Chucking depth 4. Blank part s dimensions 5. Material 6. Zero point location 7. Tool s set 1-Selecting the chuck type Module 4: CNC Programming "Turning" 31
2- Defining workpart dimensions, material and zero point 3- Selecting tool equipment 32 Module 4: CNC Programming "Turning"
The following is the automatically generated Setup Sheet: {) {{ 15.04.2008 14:47 { { CONFIGURATION { MACHINE MTS01 TM-016_-R1_-060x0646x0920 { CONTROL SINUMERIK 840DT { { PART { CYLINDER D+060.000 L+142.000 { MATERIAL "N\Aluminium\AlMg1" { DENSITY 002.70 { { MAIN SPINDLE WITH WORKPART { CHUCK "Chuck Turning\Jaw chuck\kfd-hs 130" { STEP JAW "Jaw\Step jaw\hm-110_130-02.003" { CHUCKING DEPTH E25.000 {{ Right side of the part: Z+235.000 { { TOOLS { T01 "DIN69880 V 30\Left corner tool\cl-sclcl-2020 L 1208 ISO30" { T02 EMPTY { T03 EMPTY { T04 EMPTY { T05 "DIN69880 V 30\Recessing tool\er-sgtfl-2012 L 02.0-0 ISO30" { T06 "DIN69880 V 30\Left threading tool\tl-lhtr-2020 R 60 3.50 ISO30" { T07 "DIN69880 V 30\Spotting drill\dr-15.00 034 L HSS ISO30" { T08 EMPTY { T09 "DIN69880 V 30\Twist drill\dr-15.00 067 L HSS ISO30" { T10 EMPTY { T11 EMPTY { T12 EMPTY { T13 EMPTY { T14 EMPTY { T15 EMPTY { T16 EMPTY { { TOOL COMPENSATION { D01 T01 Q3 R000.800 X+070.000 Z+045.000 G000.000 E005.005 I- 000.800 K-000.800 A+004.375 L011.855 N01 { D02 T02 Q0 R000.000 X+000.000 Z+000.000 G000.000 E000.000 I+000.000 K+000.000 A+000.000 L000.000 N01 { D03 T03 Q0 R000.000 X+000.000 Z+000.000 G000.000 E000.000 Module 4: CNC Programming "Turning" 33
I+000.000 K+000.000 A+000.000 L000.000 N01 { D04 T04 Q0 R000.000 X+000.000 Z+000.000 G000.000 E000.000 I+000.000 K+000.000 A+000.000 L000.000 N01 { D05 T05 Q3 R000.200 X+060.000 Z+041.000 G002.000 E000.000 I- 000.200 K-000.200 A+000.000 L012.000 N01 { D06 T06 Q8 R000.505 X+070.000 Z+042.699 G000.000 E000.000 I- 000.505 K+000.000 A+000.000 L000.000 N01 { D07 T07 Q7 R000.000 X+000.000 Z+106.000 G015.000 E045.000 I+000.000 K+000.000 A+000.000 L000.000 N01 { D08 T08 Q0 R000.000 X+000.000 Z+000.000 G000.000 E000.000 I+000.000 K+000.000 A+000.000 L000.000 N01 { D09 T09 Q7 R000.000 X+000.000 Z+140.000 G015.000 E059.000 I+000.000 K+000.000 A+000.000 L000.000 N01 { D10 T10 Q0 R000.000 X+000.000 Z+000.000 G000.000 E000.000 I+000.000 K+000.000 A+000.000 L000.000 N01 { D11 T11 Q0 R000.000 X+000.000 Z+000.000 G000.000 E000.000 I+000.000 K+000.000 A+000.000 L000.000 N01 { D12 T12 Q0 R000.000 X+000.000 Z+000.000 G000.000 E000.000 I+000.000 K+000.000 A+000.000 L000.000 N01 { D13 T13 Q0 R000.000 X+000.000 Z+000.000 G000.000 E000.000 I+000.000 K+000.000 A+000.000 L000.000 N01 { D14 T14 Q0 R000.000 X+000.000 Z+000.000 G000.000 E000.000 I+000.000 K+000.000 A+000.000 L000.000 N01 { D15 T15 Q0 R000.000 X+000.000 Z+000.000 G000.000 E000.000 I+000.000 K+000.000 A+000.000 L000.000 N01 { D16 T16 Q0 R000.000 X+000.000 Z+000.000 G000.000 E000.000 I+000.000 K+000.000 A+000.000 L000.000 N01 { { WORKPART ZEROPOINTS {{ Right side of the part: Z+235.000 { G54 X000.000 Z+233.000 { {) ii- Main Program: N10 G54 N15 G92 S2000 N20 G00 X150 Z150 34 Module 4: CNC Programming "Turning"
a-facing N25 T1D1 M6 N30 G96 S200 F0.2 M4 N35 G00 X65 Z0 N40 G01 X-2 N45 G01 Z2 b-parallel Turning N50 G00 X26 Z5 Module 4: CNC Programming "Turning" 35
N55 CYCLE95 ("L150",2,0,0,,0.2,0.1,0.1,1) N60 G00 X150 Z150 c- Recessing N65 T5 D1 M6 N70 G96 S125 F0.08 M4 N75 G00 X45 Z-50 N80 CYCLE93 (40,-50,5,2.5,0,0,0,-1,-1,0,0,0.2,0.3,0.5,1,5) N85 G00 X45 Z-35 N90 CYCLE93 (40,-35,5,2.5,0,0,0,-1,-1,0,0,0.2,0.3,0.5,1,5) N95 G00 X150 Z150 36 Module 4: CNC Programming "Turning"
d- Threading N100 T6 D1 M6 N110 M5 N115 G97 S1000 M3 N120 G00 X35 Z10 N125 CYCLE97 (,30,0,-15,30,30,8,0,2.15,0.02,29,0,15,3,3,1) N130 G00 X150 Z150 e- Center Drilling N135 T7 D1 M6 N140 M5 N145 G96 S100 M4 N150 G00 X0 Z5 N155 G01 Z-5 N160 G01 Z5 N165 G00 X150 Z150 Module 4: CNC Programming "Turning" 37
f- Drilling N170 T9 D1 M6 N175 G96 S1000 F0.2 M4 N180 G00 X0 Z5 N185 G01 Z-15 N190 G01 Z5 N230 G00 X150 Z150 N235 M30 Finished Part 38 Module 4: CNC Programming "Turning"
Student's Notes: Module 4: CNC Programming "Turning" 39
40 Module 4: CNC Programming "Turning"
Work Sheet Part (A): 1.Write (T) for true and (F) for false following statements: 1. The character (%) informs the controller that an NC program will follow. 2. Everything before (%) is processed by the controller. 3. The first line in an NC program is the Number (N) 4. The first line in a block is the program s name 5. An NC program is a sequence of blocks 2. Complete the following sentences: 1- The consists of a series of commands with which the CNC machine tool is instructed to manufacture a certain work part. 2- is the first word in a block. 3- The are codes determine the geometric part of the NC-program. 4- A allows performing a complete machining operation by specifying just one code. 5- Everything stands before is ignored by the control. Module 4: CNC Programming "Turning" 41
Part (B): 1. Complete the following tables: Function Description F S Tool position M3 M4 M5 Tool change Coolant OFF M30 Function Description G00 G01 G02 G03 G90 Incremental positioning 42 Module 4: CNC Programming "Turning"
Part (C): a - Write a block to move the cutting tool from starting point to target point using feed rate positioning and incremental mode. N20 N30... B - Write a command to move the tool tip from starting point to target point Using rapid positioning and absolute mode. N20 N30.. Module 4: CNC Programming "Turning" 43
C - Complete the following NC program blocks using absolute dimensioning mode. N20 N30.. D - Complete the following NC program blocks using absolute dimensioning mode. N20 N30.. 44 Module 4: CNC Programming "Turning"
Part (D): 1. What is the G code used to select the metric units of measurement? a. G21 b. G20 c. G96 d. G19 2. What is the M code used to switch on the coolant? a. M03 b. M08 c. M04 d. M09 3. What is the M code used to end a subprogram? a. M17 b. M05 c. M30 d. M02 4. In TOPTURN editor, "shift+insert" is used to: a. Delete a line b. Create a line below c. Create a line above d. None of the above 5. While programming in MTS "editor" the function is used to reorganize the blocks numbers. a. Dialog program b. Renumber c. Link programs d. WOP Module 4: CNC Programming "Turning" 45
6. Match each code with its function. Write the corresponding number in the space provided. 1 G96 Feed in mm/min. 2 M07 Constant cutting speed 3 G94 Feed in mm/rev. 4 G20 Coolant ON 5 G95 Input inch units 7. Complete the following table: Cycle Description Tapping (threading) cycle Roughing and finishing cycle Deep drilling cycle Recessing cycle 46 Module 4: CNC Programming "Turning"
Part (E) 1. Write a program to do facing by cutting only 1 mm (at Z0) for the work part shown in the figure. Given that: Work part diameter D= 50 mm Tool = T03 Constant cutting Speed = 300 m/min in counterclockwise direction. Max. spindle speed = 2000 RPM Feed = 0.2 mm/rev 2. Write a short program to produce the shape shown below: Needed: To do 1mm facing (Z=-1) then straight turning according to the drawing above, using one tool. Given: - Blank diameter 54 mm Speed limit: 2000 RPM Constant speed: 200 m/min in counterclockwise direction. Feed Rate: 0.02 mm/min. Module 4: CNC Programming "Turning" 47
N15 G54 N20 N30 N40 N50 N55 N60 N70 N80 N90 N100 N110 N120 2. Read the following NC-program carefully, then answer the questions below: N310 G54 N315 G92 S3000 N320 T1 D1 N325 G96 S200 F0.2 M4 N330 G0 X42 Z0 N335 G1 X-2 N340 G1 Z2 N345 G0 X100 Z100 N350 T2 D1 N355 G0 X20 Z5 N360 CYCLE95 ("L142",2,0,0,,0.2,0.15,0.1,1) 48 Module 4: CNC Programming "Turning"
N365 G0 X70 Z70 N370 T5 D1 N375 G0 X21 Z2 N380 M5 N385 M3 N390 CYCLE97 (,20,0,-35,20,20,10,0,1.53,,29,0,30,4,3,1) N395 G0 X100 Z100 N400 M30 1. From the program shown above, the maximum spindle speed is A.2000 RPM B.1500 RPM C.3000 RPM. D.2500RPM 2. G00 X100 Z100 Means A. tool changing point B. zero point shift C. cutting speed and feed rate rotation direction for finishing. D. constant spindle speed and rotation direction 3. In the block N360 CYCLE95 ("L142",2,0,0,,0.2,0.15,0.1,1), L142 means A. main program B. subprogram C. depth of cutting. D. tool number Module 4: CNC Programming "Turning" 49
4. Cycle 97 is used to make A. roughing B. recessing C. threading D. finishing 5. Cycle 95 could be used for A. roughing B. recessing C. threading D. taper undercut 6. M30 means A. program end B. subprogram end C. program stop D. none of the above 7. T5 D1 block is used to: A. switch the spindle on B. call tool number 5 C. compensate tool 1 D. switch the spindle off 8. The block G96 S200 F0.2 M4 stands for: A. speed limit max 200 rpm B. constant cutting speed of 200 m/min C. cutting speed limit of 2000 rpm D. speed limit min 2000 rpm 9. The G code which is used to select the work part zero point is A. G21 B. G45 C. G54 D. G50 50 Module 4: CNC Programming "Turning"
10. G01 X=-2 in a facing operation is used to: A. Change tool number 2 B. Move in rapid traverse to X=-2 C. Remove the pin at the end of the part caused by the tool tip D. Create an arc counter clockwise Part (F): a) Study the following drawing and then answer the questions below if the recessing starts from the right side. 1. Complete the missing data in the following table. Start point in X Start point in Z Width of recess Depth 2. For the second recess complete the missing data in the following table Start point in X Start point in Z Width of recess Depth Module 4: CNC Programming "Turning" 51
b) Give the listed parameters for the grooving cycle shown in the figure below: 1. Start Point in X: 70 mm 2. Start Point in Z: 60 mm 3. Groove Width: mm 4. Groove Depth: mm 5. Angle contour longitudinal axis: 6. Flank Angle Start Point: 7. Flank Angle Opposite: 8. Radius / Chamfer outside start point: mm 9. Radius / Chamfer outside opposite: mm 10. Chamfer inside start point: mm 11. Chamfer inside opposite: mm References: 1. Turning Programming Manual MTS 2. CNC technology NCADU 52 Module 4: CNC Programming "Turning"