CNC programming exmaple code which shows how a cnc machinist can use Siemens Sinumerik 840D Drilling Centering Cycle CYCLE81.
The below example code shows different methods of drilling with CYCLE81 drilling cycle.
Short Overview of SINUMERIK CYCLE81
CYCLE81 (RTP, RFP, SDIS, DP, DPR)
RTP – Return plane or Retraction plane (absolute)
RFP – Reference plane (absolute)
SDIS – Safety distance (enter without sign)
DP – Final drilling depth (absolute)
DPR – Final drilling depth relative to reference plane (enter without sign)
For detailed explanation read Sinumerik 840D CYCLE81 Drilling Centering Cycle Programming.
This programming code below use both methods of specifying final drilling depth Absolute (DP) and Relative to reference plane (DPR).
Sinumerik 840D Drilling Cycke CYCLE81 Program Example
Sinumerik 840D CYCLE81 Programming Example
N10 G0 G90 F200 S300 M3 N20 D1 T3 Z110 N21 M6 N30 X40 Y120 N40 CYCLE81(110, 100, 2, 35) N50 Y30 N60 CYCLE81(110, 102, , 35) N70 G0 G90 F180 S300 M03 N80 X90 N90 CYCLE81(110, 100, 2, , 65) N100 M30
N10 Drill speed, direction and feed etc.
N20 tool is taken to the start point in Z-axis.
N30 First drill position X40 Y120.
N40 drill will rapidly reach RFP + SDIS position 100 + 2
and will start drilling till reaches DP which is given 35
and will retract to RTP which is 110.
N50 Next drill position Y30
N60 drill will rapily reach RFP + SDIS position 102 + 0 (as SDIS is omitted).
and will start driling till reaches DP which is 35
and wil retract to RTP which is 110.
N70 Some changes in feed.
N80 Drilling position X90
N90 drill will rapidly reach RFP + SDIS position 100 + 2
As the absolute drilling depth is omitted
now cnc control will calculate final drilling depth by using Relative to reference point value (DPR)
Final drill depth (DPR) = Reference plane (RFP)position – Final Depth point position 35 (see dimension in image above)
DPR = 100 – 35
DPR = 65
