Siemens SINUMERIK 810D Programming Guide

 Siemens AG 2000. All rights reserved
0-16
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide Advanced (PGA) – 04.00 Edition
0
Preface 04.00
Structure of the manual
0
2. Detailed explanations
The theory part contains detailed information on the
following:
What is the purpose of the command?
What is the effect of the command?
What is the sequence of command?
What effect do the parameters have?
What else has to be taken into account?
The theory parts are suitable primarily as a guide for
NC beginners. Work through the manual carefully at
least once to gain an overview of the performance
scope and capabilities of your SINUMERIK control.
2
03.96 Drilling cycles and drilling patterns
2.1 Drillin
g
c
y
cles
2

Siemens AG 1997 All rights reserved.
SINUMERIK 840D/810D/FM-NC Programming Guide, Cycles (PGZ) - 08.97 Edition.
2-37
Explanation of parameters
RFP and RTP
Generally, the reference plane (RFP) and the
retraction plane (RTP) have different values. In the
cycle it is assumed that the retraction plane lies in
front of the reference plane. The distance between
the retraction plane and the final drilling depth is
therefore greater than the distance between the
reference plane and the final drilling depth.
SDIS
The safety clearance (SDIS) refers to the reference
plane. which is brought forward by the safety
clearance. The direction in which the safety
clearance is active is automatically determined by
the cycle.
DP and DPR
The drilling depth can be defined either absolute
(DP) or relative (DPR) to the reference plane.
If it is entered as an absolute value, the value is
traversed directly in the cycle.
G1
G0
RTP
RFP+SDIS
RFP
DP=RFP-DPR
X
Z
Additional notes
If a value is entered both for the DP and the DPR,
the final drilling depth is derived from the DPR. If the
DPR deviates from the absolute depth programmed
via the DP, the message "Depth: Corresponds to
value for relative depth" is output in the dialog line.
3. From theory to practice
The programming example shows you how to apply
the commands in the program.
You will find an application example for practically all
the commands after the theory part.
2
Drilling cycles and drilling patterns 03.96
2.1 Drillin
g
c
y
cles
2

Siemens AG 1997 All rights reserved.
2-38
SINUMERIK 840D/810D/FM-NC Programming Guide, Cycles (PGZ) - 08.97 Edition.
If the values for the reference plane and the
retraction plane are identical, a relative depth must
not be programmed. The error message
61101 "Reference plane incorrectly defined" is
output and the cycle is not executed. This error
message is also output if the retraction plane lies
behind the reference plane, i.e. the distance to the
final drilling depth is smaller.
Programming example
Drilling_centering
You can use this program to make 3 holes using the
drilling cycle CYCLE81, whereby this cycle is called
with different parameter settings. The drilling axis is
always the Z axis.
X
Y
40
B
90
30
0
120
35
100 108
A
A - B
Z
Y
N10 G0 G90 F200 S300 M3
Specification of the technology values
N20 D3 T3 Z110
Traverse to retraction plane
N30 X40 Y120
Traverse to first drilling position
N40 CYCLE81 (110, 100, 2, 35)
Cycle call with absolute final drilling
depth, safety clearance and incomplete
parameter list
N50 Y30
Traverse to next drilling position
N60 CYCLE81 (110, 102, , 35)
Cycle call without safety clearance
N70 G0 G90 F180 S300 M03
Specification of the technology values
N80 X90
Traverse to next position
N90 CYCLE81 (110, 100, 2, , 65)
Cycle call with relative final drilling depth
and safety clearance
N100 M30
End of program
08.97

Siemens SINUMERIK 810D Specifications

General

Brand	Siemens
Model	SINUMERIK 810D
Category	Control Unit
Language	English