Siemens SINUMERIK 828D Manual page 149
Milling with sinumerik mold-making with 3- to 5-axis simultaneous milling
Hide thumbs
Also See for SINUMERIK 828D:
- Function manual (1799 pages) ,
- Commissioning manual (1167 pages) ,
- Operating manual (926 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
subprogram:
production. Assuming that your postprocessor has been optimized, all this data should be listed
ROUGH_01
in the 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
N4590
N4595
N4600
N4610
N4620
© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
; TOOL
; T1 radius milling
tool D32 R2
G90 G17 G54
TRAFOOF
CYCLE800(1,"TC1",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,"TC1",0,57,-36,0,-105,0,0,0,0,0,0,-1)
CYCLE832(0.13,3,1)
G0 X133.1221 Y1.2413
G0 Z125
G0 Z108.1501
G1 Z103.1501 F=R1
X126.5626 Y1.1611 F=R2 ; The programmed feedrate R2 is used here
...
...
G0 Z150
CYCLE800(1,"TC1",0,57,0,0,0,0,0,0,0,0,0,-1,)
CYCLE832(0.02,0,1)
CYCLE800()
M17
; Tool specification in the form of a comment
; Tool dimensions
;
Absolute dimension specification, select
;
working plane and zero offset
; Deactivate all active transformations and
frames
; Swivel all axes to the basic 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 original 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.
;
3 roughing
;
1 as of SW 2.6.
;
;
;
; The programmed feedrate R1 is used here.
; NC blocks for geometry
; Return in Z
; Swivel to original position
; Set CYCLE832 to default values
; Resetting of the swiveled planes
; End of subprogram
6.2
149
Advertisement
Table of Contents
