BORING CYCLE (G89)

BORING CYCLE (G89)

The G89 cycle is intended for boring. This cycle uses a P number, where P specifies the number of seconds to dwell.

Program: G89 X~ Y~ Z~ A~ R~ L~ P~

The G89 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: Retract the Z-axis at the current feed rate to clear Z.

BORING CYCLE (G88)

BORING CYCLE (G88)

The G88 cycle is intended for boring and uses a P word, where P specifies the number of seconds to dwell.

Program: G88 X~ Y~ Z~ A~ R~ L~ P~

The G88 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: Stop the spindle turning.
  • Step 5: Stop the program so the operator can retract the spindle manually.
  • Step 6: Restart the spindle in the direction it was going.

BORING CYCLE (G86)

BORING CYCLE (G86)

The G86 cycle is intended for boring. This cycle uses a P number for the number of seconds to dwell.

Program: G86 X~ Y~ Z~ A~ R~ L~ P~

The G86 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: Stop the spindle turning.
  • Step 5: Retract the Z-axis at traverse rate to clear Z.
  • Step 6: Restart the spindle in the direction it was going.
  • Step 7: Move the Z-axis only at the current feed rate to the Z position.

TROUBLESHOOTING

It’s an error if:

  • The spindle is not turning before this cycle is executed

BORING CYCLE (G85)

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:

  • Step 1: Preliminary canned cycle motion.
  • Step 2: Move the Z-axis only at the current feed rate to the Z position.
  • Step 3: Retract the Z-axis at the current feed rate to clear Z.

TAPPING CYCLE (G84)

TAPPING CYCLE (G84)

The G84 cycle is intended for tapping. This cycle rotates the spindle clockwise to tap a pre-drilled hole; when the bottom of the hole is reached, the spindle rotates in the reverse direction and exits the hole.

Program: G84 X~ Y~ Z~ R~ P~ F~

  • P~ is the number of seconds to dwell
  • F~ is the feed rate

The G84 cycle is as follows:

  • Step 1: Preliminary canned cycle motion.
  • Step 2: Start the spindle forward.
  • Step 3: Move the Z-axis at the programmed feed rate (F~) to the Z-depth.
  • Step 4: Reverse the spindle.
  • Step 5: Dwell for the P number of seconds.
  • Step 6: Retract the Z-axis at the programmed feed rate (F~) to the R-plane.

This cycle uses a P word, where P specifies the number of seconds to dwell. The P word is optional – if it is not included, PathPilot calculates a dwell for you (half of a second per 1000 RPM).

Spindle speed must be commanded before calling a G84 cycle. Feed rate override is ignored during a tapping cycle. Feedhold is ignored until the return operation is executed. After the tapping operation is completed, either a G98 or G99 command controls the return height — G99 returns the tool to the R-plane; G98 returns the tool to the initial height.

Example code using G84 cycle:

N40 T51 G43 H51 M6

N45 S400 M3

N50 G54

N55 M8

N65 G0 X0.5 Y-0.75

N70 G43 Z0.6 H51

N80 G0 Z0.2

N85 S400

N90 G98 G84 X0.5 Y-0.75 Z-0.605 R0.2 F20.

N95 X1.0 Y -1.25

N100 G80

N105 G0 Z0.6

PECK DRILLING CYCLE (G83)

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~

  • 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:

  • The Q number is negative or zero

SIMPLE DRILLING CYCLE (G82)

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.

DRILLING CYCLE (G81)

DRILLING CYCLE (G81)

The G81 cycle is intended for drilling.

Program: G81 X~ Y~ Z~ A~ R~ L~

The G81 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: Retract the Z-axis at traverse rate to clear Z.

EXAMPLES

These examples demonstrate how the G81 canned cycle works in detail. Other canned cycles work in a similar manner.

EXAMPLE

The current position is (1, 2, 3), the XY-plane has been selected, and the following line of code is interpreted: G90 G81 G98 X4 Y5 Z1.5 R2.8

This means that it’s in absolute distance mode (G90), old Z retract mode (G98) and the G81 drilling cycle is performed once. The X number and X position are 4. The Y number and Y position are 5. The Z number and Z position are 1.5. The R number and clear Z are 2.8. The following moves take place:

  1. G00 motion parallel to the XY-plane to (4,5,3)
  2. G00 motion parallel to the Z-axis to (4,5,2.8)
  3. G01 motion parallel to the Z-axis to (4,5,1.5)
  4. G00 motion parallel to the Z-axis to (4,5,3)
EXAMPLE

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

CANCEL CANNED CYCLES (G80)

CANCEL CANNED CYCLES (G80)

To cancels all canned cycles, program: G80

It’s okay to program G80 if no canned cycles are in effect. After a G80, the motion mode must be set with G00 (or any other motion mode G word). If motion mode is not set after G80, this error message appears: “Cannot use axis values without a g code that uses them.”

HIGH SPEED PECK DRILL (G73)

HIGH SPEED PECK DRILL (G73)

The G73 cycle is intended for deep drilling with chip breaking. The retracts in this cycle break the chip but do not totally retract the drill from the hole. It’s suitable for tools with long flutes which clear the broken chips from the hole.

Program: G73 X~ Z~ R~ L~ Q~

  • Q~ is the delta increment along the Z-axis

The G73 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 incrementally in Z 0.010 in.
  • Step 4: Repeat Step 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:

  • The Q number is negative or zero
  • The R number is not specified