Siemens Sinumerik 840D sl Programming Manual page 85

Program code
N20 T1 D1 SVC=100
N30 X30 M3
N40 G1 X20 F0.3 G95
Example 3: Defining cutting rates for two spindles
Program code
N10 SVC[3]=100 M6 T1 D1
N20 SVC[5]=200
Example 4:
Assumptions:
Master or tool change is determined by the toolholder.
MD20124 $MC_TOOL_MANAGEMENT_TOOLHOLDER > 1
In the event of a tool change the old tool offset is retained. A tool offset for the new tool is only
activated when D is programmed:
MD20270 $MC_CUTTING_EDGE_DEFAULT = - 2
Program code
N10 $TC_MPP1[9998,1]=2
N11 $TC_MPP5[9998,1]=1
N12 $TC_MPP_SP[9998,1]=3
N20 $TC_MPP1[9998,2]=2
N21 $TC_MPP5[9998,2]=4
N22 $TC_MPP_SP[9998,2]=6
N30 $TC_TP2[2]="WZ2"
N31 $TC_DP6[2,1]=5.0
N40 $TC_TP2[8]="WZ8"
N41 $TC_DP6[8,1]=9.0
N42 $TC_DP6[8,4]=7.0
...
N100 SETMTH(1)
N110 T="WZ2" M6 D1
N120 G1 G94 F1000 M3=3 SVC=100
N130 SETMTH(4)
N140 T="WZ8"
N150 M6
Fundamentals
Programming Manual, 01/2015, 6FC5398-1BP40-5BA2
Comment
; Tool and offset data set selection together with
SVC in block (no specific sequence)
; Spindle start with CW direction of rotation, cut-
ting rate 100 m/min
; SVC and revolutional feedrate
Comment
; The tool radius of the active tool offset is the
same for both spindles. The effective speed is dif-
ferent for spindle 3 and spindle 5.
Comment
; Magazine location is toolholder
; Magazine location is toolholder 1
; Toolholder 1 is assigned to spindle 3
; Magazine location is toolholder
; Magazine location is toolholder 4
; Toolholder 4 is assigned to spindle 6
; Radius = 5.0 mm of T2, offset D1
; Radius = 9.0 mm of T8, offset D1
; Radius = 7.0 mm of T8, offset D4
; Set master toolholder number
; Tool T2 is loaded and offset D1 is activated.
; S3 = (100 m/min * 1,000) / (5.0 mm * 2 * 3.14) = 3184.71 rpm
; Set master toolholder number
; Corresponds to T8="WZ8"
; Corresponds to M4=6
Tool "WZ8" is in the master toolholder, but because MD20270=–
2, the old tool offset remains active.
Spindle motion
7.2 Cutting rate (SVC)
85