Siemens SINUMERIK 840D Manual page 95
5-axis machining
Hide thumbs
Also See for SINUMERIK 840D:
- Function manual (920 pages) ,
- Diagnostics manual (714 pages) ,
- Operating turning (713 pages)
Table of Contents
Advertisement
Complex free-form surfaces
Example roughing
The subprogram contains the NC blocks for the geometry and all the data required for produc-
subprogram:
tion. Assuming that your post processor has been optimized, all this data should be listed in the
ROUGH_01
subprogram. All subprograms are structured in a similar fashion. They only differ in terms of the
tool data, technology data, CYCLE832 parameters, and of course the NC blocks.
N100
N110
N120
N130
N140
N145
N150
N160
N170
N180
N190
N200
N210
N220
N225
N230
N240
N250
N260
N270
N280
N290
...
N4580 G0 Z150
N4590 CYCLE800(1,"K2X10F",0,57,0,0,0,0,0,0,0,0,0,-1,)
N4595
N4600 CYCLE832(0.02,10000)
N4610 CYCLE800()
N4620 M17
© Siemens AG All rights reserved. SINUMERIK, Manual, 5-axis machining
; TOOL
; T1 radius milling tool D32
R2
G90 G17 G54
TRAFOOF
CYCLE800(1,"K2X10F",0,57,0,0,0,0,0,0,0,0,0,-1,)
CYCLE800()
T1
M6
R2=10000
R1=10000
R3=4500
S10000 M3 M8
CYCLE800(0,"K2X10F",0,57,-36,0,-105,0,0,0,0,0,0,-1)
CYCLE832(0.13,112003)
G0 X133.1221 Y1.2413
G0 Z125
G0 Z108.1501
G1 Z103.1501 F=R1
X126.5626 Y1.1611 F=R2
...
...
; Tool specification in the form of a comment
; Tool dimensions
;
Absolute dimension specification, select working plane
;
and work offset
; Deactivate all active transformations and frames
; Swivel all axes to the normal position
;
Resetting of the swiveled planes for defined original
;
position
; Call tool T1
; Change tool in spindle
;
R2 as parameter for feedrate in XY plane.
;
Feedrate is programmed in NC block as R2. In this way,
;
the feedrate value can be modified quickly for the test
;
phase.
; R1 as feedrate in Z direction
; Reduced feedrate
; Spindle speed, clockwise rotation, cooling on
;
Pre-positioning of the tool in relation to the workpiece. In
;
each subprogram, a fixed position should first be
;
approached/swiveled into so that there is a defined orig-
;
inal position at the start of machining. This means that if
;
TRAORI is active, the way the workpiece is approached
;
may vary under certain circumstances. Pre-positioning
;
without TRAORI.
;
Define high speed settings with 0.13 tolerance for
;
roughing. From right to left: 3 roughing, 0 not assigned,
;
0 no TRAORI, as only 3-axis roughing, 2 G642, 1
;
FFWON SOFT, 1 COMPCAD.
;
;
;
; The programmed feedrate R1 is used here.
; The programmed feedrate R2 is used here.
; NC blocks for geometry
; Retraction in Z
; Swivel to original position
; Set CYCLE832 to default values
; Resetting of the swiveled planes
; End of subprogram
6.2
95
Hide quick links:
Advertisement
Table of Contents
