SINUMERIK 840D sl. Training. Operate - Turning (2016-2020)

M624

Contour milling programGUIDE

Sinumerik

Operate

Module Description:

This module explains the programming of a complex contour milling example with the programGUIDE

in ShopMill, by means of contour milling cycles and contour descriptions.

Module Objective:

Working with this module you learn about the technology “Contour milling”, by

programming a G code program with the programGUIDE in ShopMill.

Content:

Complex programming example

This document was produced for training purposes.

828D/840Dsl SINUMERIK Operate v4.7

Page 1

M624

Siemens assumes no responsibility for its contents.

M624

Contour milling programGUIDE

Complex programming example

Description:

A complex program (moulding plate) is to be created with the programGUIDE in ShopMill.

Objective:

The workpiece shown below is to be programmed and simulated.

Tool & technology data:

Milling cutter Ø 32 mm (CUTTER_D32)

F 0,15 mm/tooth, V 120 m/min (roughing)

F 0,08 mm/tooth, V 150 m/min (finishing)

Milling cutter Ø 16 mm (CUTTER_D16)

F 0,15 mm/tooth, V 120 m/min (roughing)

Milling cutter Ø 8.0 mm (CUTTER_D8)

F 0,10 mm/tooth, V 120 m/min (roughing)

F 0,05 mm/tooth, V 150m/min (finishing)

Operations list:

Outer contour roughing + finishing

Spigot contour roughing + finishing

Contour pocket roughing

Contour pocket rest material roughing

Contour pocket wall + base finishing

A-A

100

R36

Notes

M624

Page 4

828D/840Dsl SINUMERIK Operate

Contour milling programGUIDE

M624

Programming example: Moulding plate

The following program is to be programmed with the technology “Contour milling”.

Create a new programGUIDE program in ShopMill, with the name “DIN_CONTOURMILLING_2.MPF”.

Program the first line of the program with the following G code commands:

N10 G54 G17 G90

Insert a blank for the simulation.

Press the HSK 1.6 “Various“ to open the operating area “Various”.

Press the VSK 1 “Blank” to open the parameter window for the blank.

Insert the following parameters for the blank:

Press the VSK 8 “Accept” to confirm your inputs.

The following line is inserted into the program:

N20 WORKPIECE(,,,"BOX",64,0,-25,-80,-50,-100,100,150)

Insert now a tool call into the program.

First Press HSK 1 “Edit”. A vertical softkey-bar with additional functions shows.

Press the VSK 1.1 “Select tool”.

The “Tool selection” list window opens.

Use the blue cursor keys on the keyboard to select the tool “CUTTER_D32”.

Notes

828D/840Dsl SINUMERIK Operate

Page 5

M624

M624

Contour milling programGUIDE

Press the VSK 1.8 “OK”.

The line N30 T="CUTTER_D32" will be inserted into the program.

Alternatively you can also program this line by hand.

Program now the following G code commands:

N40 M6

N50 S1194 M3

N60 G95 FZ=0.15 ; Feedrate per tooth

Insert a contour call into the program (CYCLE62), for the “moulding plate outside”.

To do this, press the HSK 1.4 “Cont. Mill” to open the technology “Contour milling”.

Press the VSK 1 “Contour”.

Press the VSK 2 “Contour call” to open the input mask for calling up a contour in the program.

The input mask for naming the contour opens.

Fill out the name field like displayed below:

Confirm the contour name by pressing the VSK 8 “Accept”.

The following line will be inserted into the program:

N70 CYCLE62("MOULDINGPLATE_OUTSIDE",1,,)

Press VSK 2.8 to return to the VSK-bar 1.

Insert now the first “path milling cycle” (CYCLE72) into the program, for “roughing” the outside

contour.

Press the VSK 2 “Path milling” to open the input mask for the CYCLE72 “Path milling”.

Enter following values into the input mask. Use the “Select” key where indicated.

Notes

M624

Page 6

828D/840Dsl SINUMERIK Operate

Contour milling programGUIDE

M624

Confirm your inputs by pressing the VSK 8 “Accept”.

The following line will be inserted into the program:

N80 CYCLE72("",100,0,1,-15,5,0.3,0.3,0.15, 0.1,1,41,1,5,0.1,1,5,0,1,2,101,1001,100)

10.

Program now the following G code command:

N90 S1942

11.

Insert now the second path milling cycle (CYCLE72) into the program, for “finishing” the outside

contour.

Press the VSK 2 “Path milling” to open the parameter mask for the path milling cycle

(CYCLE72).

Enter following values into the input mask. Use the “Select” key where indicated.

Notes

828D/840Dsl SINUMERIK Operate

Page 7

M624

M624

Contour milling programGUIDE

Confirm your inputs by pressing the VSK 8 “Accept”.

The following line will be inserted into the program.

N100 CYCLE72("",100,0,1,-15,5,0.3,0.3,

0.08,0.1,2,41,1,5,0.1,1,5,0,1,2,101,1001,100)

12.

Insert another contour call into the program (CYCLE62), for the “spigot boundary”.

Press now the VSK 1 “Contour”.

Press the VSK 2 ”Contour call” to insert a new contour description into the program.

The input mask for naming the contour opens.

14.

Give the contour a name as shown below:

Confirm the contour name by pressing the VSK 8 “Accept”.

The following line will be inserted into the program:

N110 CYCLE62("MOULDINGPLATE_BOUNDARY",1,,)

Press VSK 2.8 to return to the VSK-bar 1.

15.

Insert another contour call (CYCLE62) into the program for the “moulding plate spigot”.

Press the VSK 1 “Contour”.

Press the VSK 2 “Contour call” to open the input mask for calling up a contour in the program.

The input mask for naming the contour opens.

16.

Give the contour a name as shown below:

Confirm the contour name by pressing the VSK 8 “Accept”.

The following line will be inserted into the program:

N120 CYCLE62("MOULDINGPLATE_SPIGOT",1,,)

Press VSK 2.8 to return to the VSK-bar 1.

17.

Insert now the first spigot milling cycle (CYCLE63), into the program, for “roughing”.

Press the VSK 6 “Spigot” to open the input mask for the CYCLE63 “Mill Spigot”.

Notes

M624

Page 8

828D/840Dsl SINUMERIK Operate

Contour milling programGUIDE

M624

18.

Enter following values into the input mask. Use the “Select”-key where indicated.

Note: With the blue “Select”-key the machining depth “Z1” can be set to “inc” or “abs” and the

tool path step over “DXY” can be set to “%” of tool Ø or as value in “mm”.

Confirm your inputs by pressing the VSK 8 “Accept”.

The following line will be inserted into the program:

N130 CYCLE63("SPIGOT",1001,100,0,1,5,0.15,,50,2.5,0.3,0,0,0,0,,,,1,2,,,,0,201,111)

19.

Insert now another spigot milling cycle (CYCLE63) into the program for “wall finishing”

Press the VSK 6 “Spigot” to open the input mask for the CYCLE63 “Mill Spigot”.

Enter following values into the input mask. Use the “Select”-key where indicated.

Confirm your inputs by pressing the VSK 8 “Accept”.

The following line will be inserted into the program:

N140 CYCLE63

("SPIGOT_FINISH_WALL",1004,100,0,1,5,0.08,,50,2.5,0.3,0,0,0,0,,,,1,2,,,,0,201,111)

Notes

828D/840Dsl SINUMERIK Operate

Page 9

M624

M624

Contour milling programGUIDE

20.

Insert now a tool call into the program.

First Press HSK 1 “Edit”. A Vertical softkey-bar with additional functions opens.

Press the VSK 1.1 “Select tool”.

The “Tool list” window opens.

Use the blue cursor keys on the keyboard to select the tool “CUTTER_D16”.

Press the VSK 1.8 “OK”.

The line N150 T="CUTTER_D16" will be inserted into the program.

Alternatively you can also program this line by hand.

21.

Program now the following G code commands:

N160 M6

N170 S2388 M3

N180 G95 FZ=0.15; Feedrate per tooth

22.

Insert another contour call (CYCLE62) into the program for the “Moulding plate pocket”.

To do this, press the HSK 1.4 “Cont. Mill” to open the technology “Contour milling”.

Press the VSK 1 “Contour”.

Press the VSK 2 “Contour call” to open the input mask for calling up a contour in the program.

The input mask for naming the contour opens.

23.

Fill out the name field like displayed below:

Confirm the contour name by pressing the VSK 8 “Accept”.

The following line will be inserted into the program:

N190 CYCLE62("MOULDINGPLATE_POCKET",1,,)

Press VSK 2.8 to return to the VSK-bar 1.

25.

Insert now a “pocket milling cycle” (CYCLE63) into the program for “roughing” the pocket.

Press the VSK 4 “Pocket” to open the input mask for the CYCLE63 “Mill pocket”.

Notes

M624

Page 10

828D/840Dsl SINUMERIK Operate

Contour milling programGUIDE

M624

Enter following values into the input mask. Use the “Select” key where indicated.

Note:

With the blue “Select”-key the machining depth “Z1” can be set to “inc” or “abs” and the tool path

step over “DXY” can be set to % of tool Ø or a value in mm of the tool Ø.

Confirm your inputs by pressing the VSK 8 “Accept”.

The following line will be inserted into the program:

N200 CYCLE63("CONTOUR_POCKET",1011,100,-

5,1,15,0.15,0.1,50,5,0.3,0.3,0,0,0,6,1.25,15,1,2,,,,0,101,111)

26.

Insert now a tool call into the program.

First Press HSK 1 “Edit”. Vertical softkey-bar with additional functions opens.

Press the VSK 1.1 “Select tool”.

The “Tool list” window opens.

Use the blue cursor keys on the keyboard to select the tool “CUTTER_D8”.

Press the VSK 1.8 “OK”.

The line N210 T="CUTTER_D8" will be inserted into the program.

Alternatively you can enter this line by hand.

27.

Program now the following G code commands:

N220 M6

N230 S4774 M3

N240 G95 FZ=0.1; Feed rate per tooth

28.

Insert now a “Pocket residual material” cycle (CYCLE63) for residual material “roughing” of the

pocket into the program.

To do this, press the HSK 1.4 “Cont. Mill” to open the technology “Contour milling”.

Press the VSK 5 “Pocket res.mat.” to open the input mask for the CYCLE63 “Pocket residual

material”.

Notes

828D/840Dsl SINUMERIK Operate

Page 11

M624

M624

Contour milling programGUIDE

Enter following values into the input mask. Use the “Select” key where indicated.

Note:

With the blue “Select”-key the machining depth “Z1” can be set to “inc” or “abs” and the tool

path step over “DXY” can be set to % of tool Ø or a value in mm of the tool Ø.

Confirm your inputs by pressing the VSK 8 “Accept”.

The following line will be inserted into the program:

N250 CYCLE63

("POCK-

ET_RESID_MAT",1001,100,0,1,20,0.1,,50,2.5,0.3,0.3,0,0,0,,,,,,"CUTTER_D16",1,,0,1101,11)

29.

Insert another pocket milling cycle (CYCLE63) into the program for “base finishing”.

Press the VSK 4 “Pocket” to open the input mask for the CYCLE63 “Mill pocket”.

30.

Program now the following G code commands:

N260 S5968

Notes

M624

Page 12

828D/840Dsl SINUMERIK Operate

Contour milling programGUIDE

M624

Enter following values into the input mask. Use the “Select” key where indicated.

Confirm your inputs by pressing the VSK 8 “Accept”.

The following line will be inserted into the program:

N270 CYCLE63

("POCK-

ET_FINISH_BASE",1003,100,0,1,20,0.05,0.1,50,5,0.3,0.3,0,0,0,6,1.25,15,1,2,,,,0,101,111)

31.

Insert another “pocket milling cycle” (CYCLE63) into the program for “Wall finishing”.

Press the VSK 4 “Pocket” to open the input mask for the CYCLE63 “Mill pocket”.

Enter following values into the input mask. Use the “Select” key where indicated.

Notes

828D/840Dsl SINUMERIK Operate

Page 13

M624

M624

Contour milling programGUIDE

Confirm your inputs by pressing the VSK 8 “Accept”.

The following line will be inserted into the program:

N280 CYCLE63

("POCK-

ET_FINISH_WALL",1004,100,0,1,20,0.05,0.1,50,5,0.3,0.3,0,0,0,6,1.25,15,1,2,,,,0,101,111)

32.

Program the following G code command to end the program:

N290 M30

33.

Now program the contour description for the “Moulding plate outside”, that you have called up

in step 7 and in the program line N70 before.

Press now the VSK 1 “Contour”.

Press the VSK ”New contour” to insert a new contour description for the machining operation.

The window for the contour name input opens. Assign the following name for the new contour.

Confirm your input by pressing VSK 8 “Accept”.

34.

The contour description window opens, where you can enter a starting point for the new con-

tour.

Enter the starting point coordinates as follows:

Confirm your inputs by pressing the VSK 8 “Accept”.

The contour description is being started and new functions to define the contour are available on

the vertical softkey bar on the right of the screen.

Notes

M624

Page 14

828D/840Dsl SINUMERIK Operate

Contour milling programGUIDE

M624

35.

Start now the contour description with the first contour element “Straight line Y”.

Press the VSK 1.3 “Straight line Y”.

The input mask for the straight line in Y-direction opens.

Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”.

The first contour element is to be created.

36.

Extend the contour now, by adding a straight line in X-direction.

Press the VSK 1.2 “Straight line X“.

The input mask for the straight line in X-direction opens.

Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”.

The contour description is extended by a new element.

37.

Finish the contour description by adding a straight line in Y-direction.

Notes

828D/840Dsl SINUMERIK Operate

Page 15

M624

Contour milling programGUIDE

M624

Finish now the contour description by pressing the VSK 8 “Accept” .

The editor window opens and the following lines will be inserted into the program:

N300 E_LAB_A_MOULDINGPLATE_OUTSIDE: ;#SM Z:2

;#7__DlgK contour definition begin - Don't change!;*GP*;*RO*;*HD*

G17 G90 DIAMOF;*GP*

G0 X-35 Y-100 ;*GP*

G1 Y35 RND=15 ;*GP*

X35 RND=15 ;*GP*

Y-100 ;*GP*

;CON,0,0.0000,3,3,MST:0,0,AX:X,Y,I,J;*GP*;*RO*;*HD*

;S,EX:-35,EY:-100;*GP*;*RO*;*HD*

;LU,EY:35;*GP*;*RO*;*HD*

;R,RROUND:15;*GP*;*RO*;*HD*

;LR,EX:35;*GP*;*RO*;*HD*

;R,RROUND:15;*GP*;*RO*;*HD*

;LD,EY:-100;*GP*;*RO*;*HD*

;#End contour definition end - Don't change!;*GP*;*RO*;*HD*

E_LAB_E_MOULDINGPLATE_OUTSIDE:

39.

Now program the contour description for the “Moulding plate pocket”, that you have called up

in step 22 and in the program line N180.

Press now the VSK 1 “Contour”.

Press the VSK ”New contour” to insert a new contour description for the machining operation.

40.

The window for the contour name input opens. Assign the following name for the new contour.

Confirm your input by pressing VSK 8 “Accept”.

41.

The contour description window opens, where you can enter a starting point for the new contour,

Notes

828D/840Dsl SINUMERIK Operate

Page 17

M624

M624

Contour milling programGUIDE

42.

Enter the starting point coordinates as follows:

Confirm your inputs by pressing the VSK 8 “Accept”.

The contour description is being started and new functions to define the contour are available

on the vertical softkey-bar on the right of the screen.

43.

Start now the contour description with the first contour element “Straight line X”.

Press the VSK 1.2 “Straight line X”.

The input mask for the straight line in X-direction opens.

Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”.

The first contour element is being created.

44.

Extend the contour now, by adding a straight line in Y-direction.

Press the VSK 1.3 “Straight line Y“.

The input mask for the straight line in Y-direction opens.

Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”.

The contour description is extended by a new element.

45.

Extend the contour now, by adding a circle in clockwise direction.

Press the VSK 1.5 “Circle“.

The input mask for the circle opens.

Notes

M624

Page 18

828D/840Dsl SINUMERIK Operate

Contour milling programGUIDE

M624

Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”

The contour description is extended by a new element.

46.

Extend the contour now, by adding a straight line in Y-direction.

Press the VSK 1.3 “Straight line Y“.

The input mask for the straight line in Y-direction opens.

Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”.

The contour description is extended by a new element.

47.

Finish the contour description by adding a straight line in X-direction.

Press the VSK 1.2 “Straight line X”

The input mask for the “Straight line X” opens.

Notes

828D/840Dsl SINUMERIK Operate

Page 19

M624

Contour milling programGUIDE

M624

Finish now the contour description by pressing the VSK 8 “Accept” .

The editor window opens and the following lines will be inserted into the program:

N310 E_LAB_A_MOULDINGPLATE_POCKET: ;#SM Z:5

;#7__DlgK contour definition begin - Don't change!;*GP*;*RO*;*HD*

G17 G90 DIAMOF;*GP*

G0 X0 Y-90 ;*GP*

G1 X30 RND=5 ;*GP*

Y-20 RND=5 ;*GP*

G2 X-30 I=AC(0) J=AC(-.1) RND=5 ;*GP*

G1 Y-90 RND=5 ;*GP*

X0 ;*GP*

;CON,0,0.0000,6,6,MST:0,0,AX:X,Y,I,J;*GP*;*RO*;*HD*

;S,EX:0,EY:-90;*GP*;*RO*;*HD*

;LR,EX:30;*GP*;*RO*;*HD*

;R,RROUND:5;*GP*;*RO*;*HD*

;LU,EY:-20;*GP*;*RO*;*HD*

;R,RROUND:5;*GP*;*RO*;*HD*

;ACW,DIA:0/235,EX:-30,EY:-20,RAD:36;*GP*;*RO*;*HD*

;R,RROUND:5;*GP*;*RO*;*HD*

;LD,EY:-90;*GP*;*RO*;*HD*

;R,RROUND:5;*GP*;*RO*;*HD*

;LR,EX:0;*GP*;*RO*;*HD*

;#End contour definition end - Don't change!;*GP*;*RO*;*HD*

49.

Now program the contour description for the “Boundary”, that you have called up in step 13

and in the program line N110.

Press now the VSK 1 “Contour”.

Press the VSK ”New contour” to insert a new contour description for the machining operation.

The window for the contour name input opens. Assign the following name for the new contour.

Confirm your input by pressing VSK 8 “Accept”.

50.

The contour description window opens, where you can enter a starting point for the new con-

tour,

Notes

828D/840Dsl SINUMERIK Operate

Page 21

M624

M624

Contour milling programGUIDE

Enter the starting point coordinates as follows:

Confirm your inputs by pressing the VSK 8 “Accept”.

The contour description is being started and new functions to define the contour are available

on the vertical softkey bar on the right of the screen.

51.

Start now the contour description with the first contour element “Straight line Y”.

Press the VSK 1.3 “Straight line Y”. The input mask for the straight line in Y-direction opens.

Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”.

The first contour element is being created.

52.

Extend the contour now, by adding a Straight line in X-direction.

Press the VSK 1.2 “Straight line X“.

The input mask for the “straight line X” opens.

Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”.

The contour description is extended by a new element.

53.

Extend the contour now, by adding a

Straight line in Y-direction.

Press the VSK 1.3 “Straight line Y”.

The input mask for the “straight line Y” opens.

Notes

M624

Page 22

828D/840Dsl SINUMERIK Operate

Contour milling programGUIDE

M624

Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”.

The contour description is extended by a new element.

54.

Finish the contour description by adding a straight line in X-direction.

Press the VSK 1.2 “Straight line X”

The input mask for the “Straight line X” opens.

Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”.

The contour description of the “Boundary” will be finished.

55.

Check now the outline of the programmed contour.

For this, use the blue cursor keys on the keyboard to place the orange selection cursor on the

symbol on the left side of the screen.

The following screen will be shown.

Notes

828D/840Dsl SINUMERIK Operate

Page 23

M624

M624

Contour milling programGUIDE

Finish now the contour description by pressing the VSK 8 “Accept” .

The editor window opens and the following lines will be inserted into the program:

N320 E_LAB_A_BOUNDARY: ;#SM Z:2

;#7__DlgK contour definition begin - Don't change!;*GP*;*RO*;*HD*

G17 G90 DIAMOF;*GP*

G0 X-30 Y-100 ;*GP*

G1 Y40 ;*GP*

X30 ;*GP*

Y-100 ;*GP*

X-30 ;*GP*

;CON,0,0.0000,5,5,MST:0,0,AX:X,Y,I,J;*GP*;*RO*;*HD*

;S,EX:-30,EY:-100;*GP*;*RO*;*HD*

;LU,EY:40;*GP*;*RO*;*HD*

;LR,EX:30;*GP*;*RO*;*HD*

;LD,EY:-100;*GP*;*RO*;*HD*

;LL,EX:-30;*GP*;*RO*;*HD*

;#End contour definition end - Don't change!;*GP*;*RO*;*HD*

E_LAB_E_BOUNDARY:

56.

Now program the contour description for the “Moulding plate spigot”, that you have called up

in step 7 and in the program line N120.

Press now the VSK 1 “Contour”.

Press the VSK ”New contour” to insert a new contour description for the machining operation.

The window for the contour name input opens. Assign the following name for the new contour:

Confirm your input by pressing VSK 8 “Accept”.

57.

The contour description window opens, where you can enter a starting point for the new

contour,

Notes

M624

Page 24

828D/840Dsl SINUMERIK Operate

Contour milling programGUIDE

M624

Enter the starting point coordinates as follows:

Confirm your inputs by pressing the VSK 8 “Accept”.

The contour description is being started and new functions to define the contour are available on

the vertical softkey bar on the right of the screen.

58.

Start now the contour description with the first contour element a “Circle” in clockwise direction.

Press the VSK 1.5 “Circle“.

The input mask for the circle opens.

Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”.

59.

Extend the contour now, by adding a Straight line in Y-direction.

Press the VSK 1.3 “Straight line Y”.

The input mask for the straight line in Y-direction opens.

Notes

828D/840Dsl SINUMERIK Operate

Page 25

M624

M624

Contour milling programGUIDE

Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”.

The contour description is extended by a new element.

60.

Extend the contour now, by adding a circle in clockwise direction.

Press the VSK 1.5 “Circle“.

The input mask for the “circle” opens.

Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”.

The contour description is extended by a new element.

61.

Extend the contour now, by adding a Straight line in Y-direction.

Press the VSK 1.3 “Straight line Y”.

The input mask for the straight line in Y-direction opens.

Notes

M624

Page 26

828D/840Dsl SINUMERIK Operate

Contour milling programGUIDE

M624

Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”.

The contour description is extended by a new element.

62.

Finish the contour description by adding a circle in clockwise direction.

Press the VSK 1.3 “Circle”

The input mask for the “Straight line X” opens.

Enter the following coordinates:

Confirm your inputs by pressing the VSK 8 “Accept”.

The contour description of the “Spigot” is now

finished.

Notes

63.

Check now the outline of the programmed contour.

828D/840Dsl SINUMERIK Operate

Page 27

M624

M624

Contour milling programGUIDE

For this, use the blue cursor keys on the keyboard to place the orange selection cursor on the

symbol on the left side of the screen.

The following screen will be shown.

Finish now the contour description by pressing the VSK 8 “Accept” .

The editor window opens and the following lines will be inserted into the program:

N330 E_LAB_A_MOLDINGPLATE_SPIGOT: ;#SM Z:5

;#7__DlgK contour definition begin - Don't change!;*GP*;*RO*;*HD*

G17 G90 DIAMOF;*GP*

G0 X0 Y-30 ;*GP*

G2 X-20 Y-22.361 I=AC(0) J=AC(0) ;*GP*

G1 Y22.361 ;*GP*

G2 X20 I=AC(0) J=AC(0) ;*GP*

G1 Y-22.361 ;*GP*

G2 X0 Y-30 I=AC(0) J=AC(-0) ;*GP*

;CON,0,0.0000,6,6,MST:0,0,AX:X,Y,I,J;*GP*;*RO*;*HD*

;S,EX:0,EY:-30;*GP*;*RO*;*HD*

;ACW,DIA:207/15,EX:-20,CX:0,RAD:30;*GP*;*RO*;*HD*

;LU,EY:22.361;*GP*;*RO*;*HD*

;ACW,DIA:7/215,EX:20,CX:0,RAD:30;*GP*;*RO*;*HD*

;LD,EY:-22.361;*GP*;*RO*;*HD*

;ACW,DIA:0/35,EX:0,EY:-30,RAD:30;*GP*;*RO*;*HD*

;#End contour definition end - Don't change!;*GP*;*RO*;*HD*

E_LAB_E_MOLDINGPLATE_SPIGOT:

Program overview “DIN_COUNTOURMILLING_2.MPF” after completion of all inputs.

N10 G54 G17 G90

N20 WORKPIECE(,,,"BOX",64,0,-25,-80,-50,-100,100,150)

N30 T="CUTTER_D32"

N40 M6

N50 S1194 M3

N60 G95 FZ=0.15

N70 CYCLE62("MOULDINGPLATE_OUTSIDE",1,,)

N80 CYCLE72("",100,0,1,-15,5,0.3,0.3,0.15,0.1,1,41,1,5,0.1,11,5,0,1,2,101,1011,100)

N90 S1942

N100 CYCLE72("",100,0,1,-15,5,0.3,0.3,0.08,0.1,2,41,1,5,0.1,1,5,0,1,2,101,1011,100)

N110 CYCLE62("BOUNDRY",1,,)

N120 CYCLE62("MOLDINGPLATE_SPIGOT",1,,)

N130 CYCLE63("SPIGOT_ROUGHING",1001,100,0,1,5,0.15,,50,2.5,0.3,0,0,0,0,,,,1,2,,,,0,201,111)

Notes

M624

Page 28

828D/840Dsl SINUMERIK Operate

Contour milling programGUIDE

M624

N140 CYCLE63("SPIGOT_FINISH_WALL",1004,100,0,1,5,0.08,,50,2.5,0.3,0,0,0,0,,,,1,2,,,,0,201,111)

N150 T="CUTTER_D16"

N160 M6

N170 S2388 M3

N180 G95 FZ=0.15

N190 CYCLE62("MOULDINGPLATE_POCKET",1,,)

N200 CYCLE63("POCKET_ROUGHING",1011,100,-5,1,15,0.15,0.1,50,5,0.3,0.3,0,0,0,6,1.25,15,1,2,,,,0,101,111)

N210 T="CUTTER_D8"

N220 M6

N230 S4766 M3

N240 G95 FZ=0.1

N250 CYCLE63("POCKET_RESID_MAT",1001,100,0,1,20,0.1,,50,2.5,0.3,0.3,0,0,0,,,,,,"CUTTER_D16",1,,0,1101,11)

N260 S5968

N270 CYCLE63("POCKET_FINISH_BASE",1003,100,0,1,20,0.05,0.1,50,5,0.3,0.3,0,0,0,6,1.25,15,1,2,,,,0,101,111)

N280 CYCLE63("POCKET_FINISH_WALL",1004,100,0,1,20,0.05,0.1,50,5,0.3,0.3,0,0,0,6,1.25,15,1,2,,,,0,101,111)

N290 M30

N300 E_LAB_A_MOULDINGPLATE_OUTSIDE: ;#SM Z:2

;#7__DlgK contour definition begin - Don't change!;*GP*;*RO*;*HD*

G17 G90 DIAMOF;*GP*

G0 X-35 Y-100 ;*GP*

G1 Y35 RND=15 ;*GP*

X35 RND=15 ;*GP*

Y-100 ;*GP*

;CON,0,0.0000,4,4,MST:0,0,AX:X,Y,I,J;*GP*;*RO*;*HD

;S,EX:-35,EY:-100;*GP*;*RO*;*HD*

;LU,EY:35;*GP*;*RO*;*HD*

;R,RROUND:15;*GP*;*RO*;*HD*

;LR,EX:35;*GP*;*RO*;*HD*

;R,RROUND:15;*GP*;*RO*;*HD*

;LD,EY:-100;*GP*;*RO*;*HD*

;#End contour definition end - Don't change!;*GP*;*RO*;*HD*

E_LAB_E_MOULDINGPLATE_OUTSIDE:

N310 E_LAB_A_MOULDINGPLATE_POCKET: ;#SM Z:5

;#7__DlgK contour definition begin - Don't change!;*GP*;*RO*;*HD*

G17 G90 DIAMOF;*GP*

G0 X0 Y-90 ;*GP*

G1 X30 RND=5 ;*GP*

Y-20 RND=5 ;*GP*

G2 X-30 I=AC(0) J=AC(-.1) RND=5 ;*GP*

G1 Y-90 RND=5 ;*GP*

X0 ;*GP*

;CON,0,0.0000,6,6,MST:0,0,AX:X,Y,I,J;*GP*;*RO*;*HD*

;S,EX:0,EY:-90;*GP*;*RO*;*HD*

;LR,EX:30;*GP*;*RO*;*HD*

;R,RROUND:5;*GP*;*RO*;*HD*

;LU,EY:-20;*GP*;*RO*;*HD*

;R,RROUND:5;*GP*;*RO*;*HD*

;ACW,DIA:0/235,EX:-30,EY:-20,RAD:36;*GP*;*RO*;*HD*

;R,RROUND:5;*GP*;*RO*;*HD*

;LD,EY:-90;*GP*;*RO*;*HD*

;R,RROUND:5;*GP*;*RO*;*HD*

;LR,EX:0;*GP*;*RO*;*HD*

;#End contour definition end - Don't change!;*GP*;*RO*;*HD*

E_LAB_E_MOULDINGPLATE_POCKET:

N320 E_LAB_A_BOUNDARY: ;#SM Z:2

;#7__DlgK contour definition begin - Don't change!;*GP*;*RO*;*HD*

G17 G90 DIAMOF;*GP*

G0 X-30 Y-100 ;*GP*

G1 Y40 ;*GP*

X30 ;*GP*

Y-100 ;*GP*

X-30 ;*GP*

;CON,0,0.0000,5,5,MST:0,0,AX:X,Y,I,J;*GP*;*RO*;*HD*

;S,EX:-30,EY:-100;*GP*;*RO*;*HD*

;LU,EY:40;*GP*;*RO*;*HD*

;LR,EX:30;*GP*;*RO*;*HD*

;LD,EY:-100;*GP*;*RO*;*HD*

;LL,EX:-30;*GP*;*RO*;*HD*

;#End contour definition end - Don't change!;*GP*;*RO*;*HD*

E_LAB_E_BOUNDARY:

Notes

828D/840Dsl SINUMERIK Operate

Page 29

M624

M624

Contour milling programGUIDE

N330 E_LAB_A_MOLDINGPLATE_SPIGOT: ;#SM Z:5

;#7__DlgK contour definition begin - Don't change!;*GP*;*RO*;*HD*

G17 G90 DIAMOF;*GP*

G0 X0 Y-30 ;*GP*

G2 X-20 Y-22.361 I=AC(0) J=AC(0) ;*GP*

G1 Y22.361 ;*GP*

G2 X20 I=AC(0) J=AC(0) ;*GP*

G1 Y-22.361 ;*GP*

G2 X0 Y-30 I=AC(0) J=AC(-0) ;*GP*

;CON,0,0.0000,6,6,MST:0,0,AX:X,Y,I,J;*GP*;*RO*;*HD*

;S,EX:0,EY:-30;*GP*;*RO*;*HD*

;ACW,DIA:207/15,EX:-20,CX:0,RAD:30;*GP*;*RO*;*HD*

;LU,EY:22.361;*GP*;*RO*;*HD*

;ACW,DIA:7/215,EX:20,CX:0,RAD:30;*GP*;*RO*;*HD*

;LD,EY:-22.361;*GP*;*RO*;*HD*

;ACW,DIA:0/35,EX:0,EY:-30,RAD:30;*GP*;*RO*;*HD*

;#End contour definition end - Don't change!;*GP*;*RO*;*HD*

E_LAB_E_MOLDINGPLATE_SPIGOT:

64.

Start the simulation of the program.

Press the HSK 1.7 “Simulation” to open the simulation window.

The control calculates the simulation and shows the simulation by default in the “top view”.

Press the VSK 1.4 “3D view“ to run the simulation in a 3D view.

M624: END

Notes

M624

Page 30

828D/840Dsl SINUMERIK Operate

M572

Operating mode “AUTO”

Sinumerik

Operate

Module Description:

This module describes, how to overstore technological parameters (for example, auxiliary

functions, axis feed, spindle speed, programmable instructions, etc.) for a program run in the

main memory of the NCK.

It is described among other things, how the execution of a program can be stopped at a specific part

of the program run with the function “Program control“ (programmed stop).

The differences between the two block search modes (with or without calculation) will be explained in

detail as well as the function “Simultaneous recording”.

Module Objective:

In this module you learn the different options of the operating mode "AUTO" in the oper-

ating area "Machine".

Content:

Operating mode “AUTO“

Overstore

Program control

Block search

Simultaneous recording

Program correction

Settings

This document was produced for training purposes.

828D/840Dsl SINUMERIK Operate v4.7

Page 1

M572

Siemens assumes no responsibility for its contents.

M572

Operating mode “AUTO”

Operating mode “AUTO

Selecting the operating mode “AUTO”

The operating mode “AUTO” can be selected as follows:

Press the “AUTO“ button on the machine control panel (MCP).

The operating mode “AUTO” opens directly.

- OR -

Press the button “MENU SELECT“ on the machine control panel.

Press the VSK 1 “AUTO“ in the yellow VSK-bar on the right hand side of the screen to switch

directly to the operating mode “AUTO“.

Next, switch to the operating area “Machine” by pressing the “MACHINE”-key on the operator

panel or the keyboard else press the “MENU SELECT“ key on the operator panel and the

yellow HSK 1 “Machine“.

The following screen opens:

The following softkeys will be shown in the vertical and horizontal softkey bars:

Vertical softkey bar 1 and 2

Display area

Description

By pressing the VSK 1.1 “G functions“ the most important G-functions will be displayed.

By pressing the VSK 1.2 “Auxiliary functions“, available auxiliary functions will be displayed

at the time of the output.

By pressing the VSK 1.3 “Basic blocks“ all G-code commands that trigger a function on the

machine will be displayed. The display updates both in the test operation and in the actual

machining of the workpiece at the machine.

Notes

M572

Page 4

828D/840Dsl SINUMERIK Operate

Operating mode “AUTO”

M572

Display area

Description (continuation)

By pressing the VSK 1.4 “Time / counter“ the program run time, the rest of the program run

time and the amount of machined workpieces will be displayed.

Note: Refer to the machine manufacturer’s documentation.

By pressing the VSK 1.5 “Program levels“ you can display the current program level during the

execution of a large program with several subprograms.

By pressing the VSK 1.7 “Act values. Machine” you can switch over from the machine coordi-

nate system (MCS) to the workpiece coordinate system (WCS).

Note:

Refer to the machine manufacturer’s documentation.

By pressing the VSK 1.8 "Extend" on the operator panel (OP) you switch to the vertical softkey

bar 2 with additional softkeys displayed.

By pressing the VSK 2.2 “All G functions” all G-functions will be displayed.

By pressing the VSK 2.6 “Zoom act. val.“ all actual values will be displayed full-screen.

By pressing the VSK 2.8 “Back” on the operator panel you can switch back to the vertical soft-

key bar 1.

Horizontal softkey bar 1 and 2

Display area

Description

Pressing the HSK 1.2 “Overstore” allows you to overstore technological parameters (for exam-

ple, auxiliary functions, axis feed, spindle speed, programmable instructions, etc.) for a program

run in the main memory of the NCK.

By pressing the HSK 1.4 “Prog. cntrl.” the working window for controlling the program run will

be opened.

By pressing the HSK 1.5 “Block search” the block search window opens.

By pressing the HSK 1.7 “Simultaneous record.“ you can graphically display the execution of

the program on the screen before or during machining of the workpiece, to monitor the result of

the programming.

By pressing the HSK 1.8 “Prog. corr.“ (program correction) the program editor opens.

By pressing the "Extend"-button on the operator panel you can switch between the normal and

the extended horizontal softkey bar.

This symbol on the right of the dialogue line indicates that more softkeys are available on the

extended horizontal softkey bar.

This symbol indicates that the extended horizontal softkey bar is shown on the screen. You can

switch back to the HSK 1 again by pressing the “Extend” key.

Notes

828D/840Dsl SINUMERIK Operate

Page 5

M572

M572

Operating mode “AUTO”

Display area

Description (continuation)

By pressing the HSK 2.6 "Handwheel" the input mask for assigning axes to all parameterized

handwheels is displayed.

By pressing the HSK 2.7 "Synchr. Action." the screen which shows the current synchronized

actions is displayed.

By pressing the HSK 2.8 "Settings" a window opens up where you can adjust the settings for

manual operation on the Sinumerik Operate.

Overstore

Selecting the Function “Overstore“

By pressing the HSK 1.2 “Overstore“ the “Overstore” window opens (see picture below).

The program to be corrected has to be in the STOP or RESET mode.

In the “Overstore” editor view you can overstore technological parameters (for example, auxiliary functions, axis feed, spin-

dle speed, programmable instructions, etc.) for a program run in the main memory of the NCK.

The programs in the part program memory are not changed while using the function “Overstore”.

You cannot change the operating mode while you are in overstore mode.

Notes

M572

Page 6

828D/840Dsl SINUMERIK Operate

Operating mode “AUTO”

M572

Vertical softkey bar

Display area

Description

By pressing the VSK 1.5 “Delete blocks” you can delete the blocks you have entered before.

By pressing the VSK 1.8 “Back“ the window is being closed. A change of the operation mode is

now possible. Press “CYCLE START“ to continue running the previously selected program.

Procedure for “Overstore“

Open a program in the operating mode “AUTO” then press the HSK 1.2 “Overstore”. The “Overstore” window

opens.

Enter the required data and NC block.

Press the “CYCLE START” key. The blocks you have entered are stored. You can observe execution in the

"Overstore" window. After the entered blocks have been executed, you can append blocks again.

Press the VSK 8 "Back". The "Overstore" window closes.

Press the “CYCLE START” key again.

The program selected before overstoring continues to run.

Program control

Selecting the function “Program control”

By pressing the HSK 1.4 “Prog. cntrl.“ the “Program control” window opens like displayed

below:

Notes

828D/840Dsl SINUMERIK Operate

Page 7

M572

M572

Operating mode “AUTO”

Navigation through the option menu takes place by pressing the blue Cursor keys on the key-

board.

You can activate or deactivate an option by selecting the entry first and then pressing the blue

“SELECT“ key.

The following program control options are selectable:

Abbreviation/Program

Scope

control

PRT

The program is started and executed with auxiliary function outputs and dwell times. In this

No axis motion

mode, the axes are not traversed.

The programmed axis positions and the auxiliary function outputs are controlled this way.

Note:

Program processing without axis motion can also be activated with the function "Dry run

feedrate".

DRY

The traversing velocities programmed in conjunction with G1, G2, G3, CIP and CT are replaced

Dry run feedrate

by a defined dry run feedrate. The dry run feedrate also applies instead of the programmed

revolutional feedrate.

Caution:

Workpieces must not be machined when "Dry run feedrate" is active because the altered

feedrates might cause the permissible tool cutting rates to be exceeded and the workpiece or

machine tool could be damaged.

RG0

In the rapid traverse mode, the traversing speed of the axes is reduced to the percentage value

Reduced rapid trav.

entered in RG0.

M01

The processing of the program stops at every block in which supplementary function “M01” is

Programmed stop 1

programmed. In this way you can check the already obtained result during the processing of a

workpiece.

Note:

In order to continue executing the program, press the "CYCLE START" key again.

Programmed stop 2

The processing of the program stops at every block in which the "Cycle end" is programmed

(e.g. M201)

(e.g. with “M201”).

Note:

In order to continue executing the program, press the "CYCLE START" key again.

The display can be changed. Please also refer to the machine manufacturer's instructions.

DRF

Enables an additional incremental zero offset while processing in automatic operation mode

Handwheel offset

with an electronic handwheel.

This function can be used to compensate for tool wear within a programmed block.

Individual blocks are configured as follows:

 SB 1 - Single block, coarse: The program stops only after blocks which perform a machine

function.

 SB 2 - Data block: The program stops after each block.

 SB 3 - Single block, fine: The program stops also in cycles after blocks, which perform a

machine function.

Select the desired setting using the "SELECT" key on the keyboard.

The selection of the function “Single block” takes place by pressing the “SINGLE BLOCK”-key

on the machine control panel (MCP).

SKP

Skipped blocks are skipped during machining.

MRD

In the program, the measurement results screen display is active while machining.

Notes

M572

Page 8

828D/840Dsl SINUMERIK Operate

Operating mode “AUTO”

M572

Vertical softkey bar

Display area

Description

By pressing the VSK 8 “Back” you return to the window “Program control”.

Controlling the program run

In the operating mode “AUTO“ and the operating area “Machine” press the HSK 4 “Prog.

cntrl.“.

The “Program control” window opens and shows a list of program control options.

Select the desired program control.

Press the VSK 8 “Back” to go back to the main screen of the Sinumerik Operate in the operat-

ing mode “AUTO” and operating area “Machine”.

Block search

Selecting the function “Block search”

By pressing the HSK 1.5 “Block search” the “block search” window opens as shown below.

Notes

828D/840Dsl SINUMERIK Operate

Page 9

M572

M572

Operating mode “AUTO”

If you would only like to perform a certain section of a program on the machine, then you don’t have to start the program

from the beginning. You can also start the program from a specified program block.

Applications of this function are to stop or interrupt program execution and to specify a target position (e.g. during

machining).

Determination of search targets per:

a. Easy search target definitions (search positions)

 Direct specification of the search target by positioning the cursor in the selected program (main program).

 Search target via text search.

 The search target is the interruption point (main program and subprogram). The function is only available if there is an

interruption point. After a program interruption (“CYCLE STOP” or “RESET”), the controller saves the coordinates of the

interruption point.

 The search target is the higher program level of the interruption point (main program and subprogram). The level can

only be changed if it was previously possible to select an interruption point in a subprogram. It is then possible to

change the program level up to the main program level and back to the level of the interruption point.

OR -

b. Search pointer

 Direct entry of the program path in the “Search pointer“ window.

If a search target was found, it is possible to start another search run immediately. This can be done many times after

every successful search run.

Attention:

Pay attention to a collision-free starting position as well as accurate active tools and other technological values. If neces-

sary move the tool to a save starting position. Select the target block considering the selected block search type.

Navigation through the program blocks takes place by using the blue cursor-keys on the

keyboard.

The following functions are available in the vertical softkey bar:

Notes

M572

Page 10

828D/840Dsl SINUMERIK Operate

Operating mode “AUTO”

M572

Vertical softkey bar

Display area

Description

By pressing the VSK 1 “Start search“ the search run starts depending on the search mode you

have selected before. Press the VSK 1 several times, until the found target (e.g. with search

text) corresponds to the searched program block.

By pressing the VSK 2 “Blk. sear. mode“ the “Block search mode” window opens.

Two different block search modes are selectable:

With calculation:

 Without approach:

It is used in order to be able to approach a target position in any circumstance (e.g. tool

change position). The end position of the target block or the next programmed position is

approached using the type of interpolation valid in the target block. Only the axes

programmed in the target block are moved.

 With approach:

It is used to be able to approach the contour in any circumstance. The end position of the

block prior to the target block is found with "CYCLE START". The program runs in the same

way as in normal program processing.

Display area

Description (continuation)

Without calculation:

 For a quick search in the main program. Calculations will not be performed during the block

search, i.e. the calculation is skipped up to the target block. All settings required for

execution have to be programmed from the target block (e.g. feedrate, spindle speed, etc.).

Pressing the VSK 3 “Higher level“ changes the program level to one level higher.

Pressing the VSK 4 “Lower level“ changes the program level to one level lower.

By pressing the VSK 5 “Search for text“ the “Search” window opens. After entering the search

direction in the “Direction” field and the search text in the “Text” field and by pressing the VSK 8

“OK” the search run starts. After a successful search you can search for the same search pa-

rameter again, by pressing the VSK 8 “Continue search”.

The search can be cancelled by pressing the VSK 7 “Cancel”. A new search run with new

search parameters can be initiated with the VSK 4 “Search”.

By pressing the VSK 6 “Interrupt point” the program that was interrupted before, by pressing

the “RESET” key, will be executed again.

By pressing the VSK 7 “Search pointer“ you can jump directly to a desired part of the program.

The following options are available in a list in the “Search pointer” window:

 Program

The name of the currently loaded program is automatically entered

 Ext.

File extension

 P

Pass counter: If a program section is performed several times, you can enter the number of

the pass here at which processing is to be continued

 Line

Is automatically filled for an interruption point

Notes

828D/840Dsl SINUMERIK Operate

Page 11

M572

M572

Operating mode “AUTO”

Display area

Description (continuation)

 Type

 N no.:

Block number

 Label:

Jump label

 Text:

Text string

 Subprg.:

Subprogram call

 Line:

Line number

 Search target

Search target point in the program at which machining is to start

By pressing the VSK 8 “Back” the “Search” window closes.

Starting a block search

A desired program is selected and the machining was discontinued with pressing “RESET” or

“CYCLE STOP“ or the control unit is generally in RESET state.

In the operating mode “AUTO“ and the operating area “Machine” press the HSK 5 “Block

search”.

For further steps see below:

Simple search target definition:

Steps 1 and 2 (see above).

Place the cursor on a particular program block.

- OR -

Press the VSK 5 "Search for text", select the search direction, enter the search text and con-

firm with the VSK 8 "OK".

Press the VSK 1 “Start search“.

The search starts.

Your specified search mode will be taken into account (indicated in the upper blue title bar of

the search target window). The current block will be displayed and marked in the "Program"

window as soon as the target is found.

If the located target (for example, when searching via text) does not correspond to the pro-

gram block, press the "Start search" softkey again until you find your target.

Press the "CYCLE START"-key twice.

Processing is continued from the defined position.

Notes

M572

Page 12

828D/840Dsl SINUMERIK Operate

Operating mode “AUTO”

M572

Interruption point as search target:

1. - 2.

Steps 1 and 2 (see above).

Press the VSK 6 “Interrupt point“

The interruption point is loaded.

If the VSK 3 "Higher level" and the VSK 4 "Lower level" are available, use these to change the

program level.

Press the VSK 1 "Start search".

The search starts.

The specified search mode will be taken into account (indicated in the upper blue title bar of the

search target window).

The search screen closes.

The current block will be displayed and marked in the "Program" window as soon as the target

is found.

Press the "CYCLE START"-key on the machine control panel (MCP) twice.

The execution will continue from the interruption point.

Search target via search pointer:

Steps 1 and 2 (see above).

Press the VSK 7 “Search pointer”.

The “Search pointer” window opens.

Enter the full path of the program as well as the subprograms, if required, in the input fields.

Press the VSK 1 “Start search”.

The search starts.

The specified search mode will be taken into account (indicated in the upper blue title bar of the

search target window).

The search screen closes.

The current block will be displayed and marked in the "Program" window as soon as the target

is found.

Press the "CYCLE START" key on the machine control panel twice.

Processing is continued from the defined location.

Notes

828D/840Dsl SINUMERIK Operate

Page 13

M572

M572

Operating mode “AUTO”

Simultaneous recording

Selecting the function “Simultaneous recording”

Pressing the HSK 1.7 “Simult. Record.“ opens the simultaneous recording window.

Before machining the workpiece on the machine, you can graphically display the execution of the program on the screen to

monitor the result of the programming. You can replace the programmed feedrate with a dry run feedrate to influence the

speed of execution.

Simultaneous record can also be turned on, if machining is already running. You can also use simultaneous recording

during machining of a workpiece. This helps if the view towards the inside of the cabin is obstructed by coolant. In each

different view of the “Simultaneous recording” window you can adjust the view by using the blue cursor keys and zoom in or

out by using the plus (“+”) and minus (“-”) keys on the keyboard.

The traversing paths of the tool in the “Simultaneous recording” window are displayed in different colours: red for rapid

Simultaneous recording of a program run

Simultaneous recording before machining of the workpiece

Load a program in the operating mode “AUTO”.

Press the HSK 1.4 “Prog. cntrl.“ and activate the checkboxes "PRT No axis motion" and "DRY

Dry run feedrate".

The program is executed without axis movement. The programmed feedrate is replaced by a dry

run feedrate.

-OR-

Let the “DRY Dry run feedrate” box unchecked.

Simultaneous recording is performed with the programmed feedrate.

Press the HSK 7 “Simult. record.“.

The “Simultaneous recording” window opens.

Press the “CYCLE START” key on the machine control panel (MCP).

The execution of the program on the machine is started and displayed graphically on the screen.

Press “CYCLE STOP” to stop machining and the HSK 7 "Simult. record." again to close the

“Simultaneous recording” window.

Notes

M572

Page 14

828D/840Dsl SINUMERIK Operate

Operating mode “AUTO”

M572

Simultaneous recording during machining of the workpiece

Load a program in the operating mode “AUTO”.

Press the HSK 7 “Simult. record.“.

The “Simultaneous recording” window opens.

Press the “CYCLE START”-key on the machine control panel (MCP).

The machining of the workpiece is started and graphically displayed on the screen.

Press the “CYCLE STOP”-key and the HSK 7 "Simult. record." again to stop the recording and

to close the “Simultaneous recording” window.

As soon as a syntax error in the part program is detected by the controller, program execution is interrupted and the syntax

error is displayed in the alarm line.

Depending on the state of the control, you can make the following corrections using the “Program correction” function:

 STOP mode: Only program lines that have not yet been executed can be edited.

 RESET state: All program lines can be edited

Note:

The "Program correction" function is only available for part programs in the NC memory, not for external execution (e.g.

on USB media).

Program correction

Selecting the function “Program correction”

By pressing the HSK 1.8 “Prog. Corr.“ the program editor window opens for correction of the

program.

Notes

828D/840Dsl SINUMERIK Operate

Page 15

M572

M572

Operating mode “AUTO”

Vertical softkey bar 1 and 2

A precise description of the vertical softkeys can be found in the modules B600 and B604 “Basics of programming”.

Settings

Selecting the function “Settings”

By pressing the HSK 2.8 “Settings” the following input mask with the settings for automatic

mode is shown on the screen.

Vertical softkey bar (VSK)

Display area

Description

By pressing the VSK 5 "Changeover inch" the measuring units are converted from the metric

to the imperial (inch) dimension system. New values have to be entered in inches. By press-

ing this key the key function switches to "Changeover metric".

By pressing the VSK 5 "Changeover metric" the measuring units are converted from the

imperial (inch) to the metric dimension system. New values have to be metric. By pressing this

key the key function switches to "Changeover inch".

Accept the selection by pressing the VSK 8 “OK” or

cancel by pressing the VSK 7 “Cancel”.

By pressing the VSK 8 "Back" you switch back to the main screen of the Sinumerik Operate.

Parameters for "Settings for automatic mode"

In the “Settings for automatic mode“ window all configurations for automatic operation can be done.

Parameter

Unit

Meaning

Dry run feedrate

[mm/ min] The feedrate defined here replaces the programmed feedrate during execution if you

have selected „DRY dry run feedrate“ under program control.

DRY

Reduced rapid traverse

[%]

This value entered here reduces the rapid traverse to the entered percentage value if

RG0

you have selected “RG0 reduced rapid traverse” under program control.

Record machine time

The machining times are determined for each block of the main program or deter-

mined for all blocks and shown in the “Working window”, this function can also be

switched off.

Save machining times

A time stamp is placed into the NC program and stored for future reference, or this

function can be switched off.

M572: END

Notes

M572

Page 16

828D/840Dsl SINUMERIK Operate

M560

Mirror, offset, rotate, scale

Shifting

General introduction

The commands in this module are known as frames (calculation instructions). They can influence, cancel or condition each

other. In our example a known contour, which is described in a subprogram, is to be milled in various positions and sizes.

“TRANS”, “ATRANS”

The zero point can be shifted in the programmed axes by means of these commands. The command “TRANS” clears all

active frames. “ATRANS” (additive shift) works incremental from the active frames.

Workpiece 1

Workpiece 2

Workpiece 3

Workpiece 4

ATRANS x30

TRANS x60

ATRANS x30

For instance in case of multiple settings of work pieces the zero point can be shifted and the main program repeatedly exe-

cuted .

Rotating

“ROT”, “AROT”

The coordinate system can be rotated by means of the command “ROT” or “AROT”. The counter-clockwise rotation is tak-

en to be positive. The positive X-axis represents the zero-degree position.

There are two ways of programming.

Variant 1

Rotation about an axis AROT X.. Y.. Z..

AROT Z=90

X+

The zero point has been rotated by 90° about the Z-axis.

Variant 2

Rotation of the active plane AROT RPL...

AROT RPL=90

X+

The active plane has been rotated by 90° about the Z-axis.

The command “ROT” resets the coordinate system and all other active frames back to the original status.

Notes

M560

Page 4

828D/840Dsl SINUMERIK Operate

Mirror, offset, rotate, scale

M560

Mirroring

“MIRROR”, “AMIRROR”

With the command “MIRROR” or “AMIRROR” the coordinate system can be mirrored about the programmed axis or axes.

In such a case the programmed coordinates are mirrored about the axis or axes by their sign.

Variant 1

Mirroring an axis

AMIRROR X0

X+

Variant 2

Mirroring several axes

MIRROR X0 Y0

X+

Scaling

“SCALE”, “ASCALE”

In some cases the scaling of contour elements is quite sensible. The existing contours can be scaled up or down by a given

factor.

The factor is defined following the command Scale for each individual axis.

SCALE y2

SCALE x2

SCALE x2 y2

ASCALE y2

ASCALE x2

SCALE

When programming with “ASCALE” the calculations are always referred to the presently valid coordinate system. With the

command “SCALE” the values of the active zero point offset are taken as a basis. All presently active transformations

(frames) like offset, mirror, scale are cancelled.

If no value follows the command “SCALE” all frames are cancelled. The same applies to the command “M30”.

Notes

828D/840Dsl SINUMERIK Operate

Page 5

M560

M560

Mirror, offset, rotate, scale

The value programmed under “SCALE” represents a factor. If this is >1 an enlargement takes place, in case of values <1

diminished. Care must be taken that radii are also affected. This can possibly lead to errors.

Variant 1

........Scaling of an axis

ASCALE X1.5

All X-values are multiplied by 1.5

Variant 2

.......Scaling of several axes

ASCALE X=1x1.5 Y=1x1.5

The scaling factor can also be calculated in the program by entering the formula.

Summary

Frame - Concept (Calculation instructions)

TRANS X... Y... Z...

Absolute programmable zero point offset as referred to the presently valid, with G54 to G57

and G505 to G599 selected work piece zero point

ATRANS X... Y... Z...

Additive programmable zero point offset as referred to the presently valid, selected or pro-

grammed zero point

Shift value in direction of the stated axis

TRANS

Deactivation of programmable zero point offsets, previously programmed frames are cleared

ROT X.. Y.. Z.. RPL=..

Absolute programmable rotation as referred to the presently valid, with G54 to G57 and G505

to G599 selected work piece zero point

AROT X.. Y.. Z.. RPL=..

Additive programmable rotation as referred to the presently valid, selected or programmed

zero point

Rotation angle in space: - Geometry axis that is being rotated

RPL=

Rotation angle in a plane: - angle by which the coordinate system Is rotated - (plane previously

selected with G17 to G19)

ROT

Deactivation of programmable rotation, previously programmed frames are cleared

SCALE X... Y... Z...

Absolute programmable enlarging or diminishing (scaling), as referred to the presently valid,

with G54 to G57 and G505 to G599 selected work piece zero point

ASCALE X... Y... Z...

Additive programmable enlarging or diminishing (scaling) as referred to the presently valid,

selected or programmed zero point

Scaling factor (smaller / greater 1) in direction of stated axis

SCALE

Deactivation of programmable enlarging or diminishing, previously programmed frames are

cleared

MIRROR X... Y... Z...

Absolute programmable mirroring as referred to the presently valid, with G54 to G57 and

G505 to G599 selected work piece zero point

AMIRROR X...Y...Z...

Additive programmable mirroring as referred to the presently valid, selected or programmed

zero point

Coordinate axis, in which the signs are changed, (the value for X/Y or Z can be freely selected

- e. g. X0/Y0/Z0)

MIRROR

Deactivation of programmable mirroring, previously programmed frames are cleared

M560: END

Notes

M560

Page 6

828D/840Dsl SINUMERIK Operate

M700

Drawings of programming examples

Sinumerik

Operate

Module Description:

This module contains all the drawings that were used in the individual modules so far and additional

work piece drawings as exercises for the consolidation of the acquired knowledge.

Module Objective:

This module provides the means to carry out further exercises regarding the programming with Shop-

Mill and to consolidate the programming knowledge so far attained.

Content:



Shop drawings

- Mould

- Moulding plate

- Guide plate_1

- Housing cover

- Perforated plate

- Exhibition example

- Longitudinal guide

- Mould plate_2

- Flange

- Exercise_12

- Guide plate_2

- Kidney-shaped plate

- Mould plate

- Example_1

- Mould_2

- Pressure plate

- Con-rod

- Wing

- Connecting piece

This document was produced for training purposes.

828D/840Dsl SINUMERIK Operate v4.5

Page 1

M700

Siemens assumes no responsibility for its contents.

SINUMERIK 840D sl. Training. Operate - Turning (2016-2020) - page 19