9: PROGRAMMING
E X A M P L E
The current position is (1, 2, 3), the XY-plane has been
selected, the following line of code is interpreted: G91
G81 G98 X4 Y5 Z-0.6 R1.8 L3
This means that it's in incremental distance mode
(G91), old Z retract mode, and the G81 drilling cycle is
repeated three times. The X number is 4, the Y number
is 5, the Z number is -0.6 and the R number is 1.8. The
initial X position is 5 (=1+4), the initial Y position is 7
(=2+5), the clear Z position is 4.8 (=1.8+3) and the Z
position is 4.2 (=4.8-0.6). Old Z is 3.0.
The first move is a traverse along the Z-axis to (1,2,4.8),
since old Z < clear Z.
The first repeat consists of three moves:
1. G00 motion parallel to the XY-plane to (5,7,4.8)
2. G01 motion parallel to the Z-axis to (5,7, 4.2)
3. G00 motion parallel to the Z-axis to (5,7,4.8)
The second repeat consists of three moves. The X
position is reset to 9 (=5+4) and the Y position to 12
(=7+5):
1. G00 motion parallel to the XY-plane to (9,12,4.8)
2. G01 motion parallel to the Z-axis to (9,12, 4.2)
3. G00 motion parallel to the Z-axis to (9,12,4.8)
The third repeat consists of three moves. The X position
is reset to 13 (=9+4) and the Y position to 17 (=12+5):
1. G00 motion parallel to the XY-plane to (13,17,4.8)
2. G01 motion parallel to the Z-axis to (13,17, 4.2)
3. G00 motion parallel to the Z-axis to (13,17,4.8)
Example code using G81 cycle:
(Sample Program G81EX18:)
(Workpiece Size: X4, Y3, Z1)
(Tool: Tool #6, 3/4” HSS DRILL)
(Tool Start Position: X0, Y0, Z1)
N2 G90 G80 G40 G54 G20 G17 G94 G64 (Safety Block)
N5 G90 G80 G20
N10 M06 T6 G43 H6
N15 M03 S1300
N20 G00 X1 Y1
N25 Z0.5
N30 G81 Z-0.25 R0.125 F5 (Drill Cycle Invoked)
N35 X2
N40 X3
N45 Y2
N50 X2
N55 X1
N60 G80 G00 Z1 (Cancel Canned Cycles)
N65 X0 Y0
N70 M05
N75 M30
9.3.5 Simple Drilling Cycle (G82)
The G82 cycle is intended for drilling.
Program: G82 X~ Y~ Z~ A~ R~ L~ P~
The G82 cycle is as follows:
Step 1: Preliminary canned cycle motion.
Step 2: Move the Z-axis only at the current feed
rate to the Z position.
Step 3: Dwell for the P number of seconds.
Step 4: Dwell for the P number of seconds.
9.3.6 Peck Drilling Cycle (G83)
The G83 cycle (often called peck drilling) is intended for deep
drilling or milling with chip breaking. The retracts in this cycle
clear the hole of chips and cut off any long stringers (which are
common when drilling in aluminum).
Program: G83 X~ Y~ Z~ A~ R~ L~ Q~
l Q~ is a delta increment along the Z-axis
The G83 cycle is as follows:
Step 1: Preliminary canned cycle motion.
Step 2: Move the Z-axis only at the current feed
rate downward by delta or to the Z position,
whichever is less deep.
Step 3: Rapid back out to the clear Z.
Step 4: Repeat Steps 1 through 3 until the Z
position is reached at Step 1.
Step 5: Rapid back down to the current hole
bottom, backed off a bit.
Step 6: Retract the Z-axis at traverse rate to clear
Z.
Troubleshooting
It's an error if:
l The Q number is negative or zero
9.3.7 Boring Cycle (G85)
The G85 cycle is intended for boring or reaming, but could be
used for drilling or milling.
Program: G85 X~ Y~ Z~ A~ R~ L~
The G85 cycle is as follows:
©Tormach® 2024
Specifications subject to change without notice.
Page 191 UM10811: 1500MX Operator's Manual (Version 0424A)
For the most recent version, see tormach.com/support
To Next Page
Loading...
