FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. For Machining Center System USER’S MANUAL - page 3
5. FUNCTIONS TO SIMPLIFY
PROGRAMMING
PROGRAMMING
B-64304EN-2/01
Limitation
- Axis switching
Before the drilling axis can be changed, the canned cycle for drilling
must be canceled.
- Drilling
In a block that does not contain X, Y, Z, R, or any other axes, drilling
is not performed.
- Cancel
Do not specify a G code of the 01 group (G00 to G03) and G81 in a
single block. Otherwise, G81 will be canceled.
- Tool offset
In the canned cycle mode for drilling, tool offsets are ignored.
Example
M3 S2000 ;
Cause the spindle to start rotating.
G90 G99 G81 X300. Y-250. Z-150. R-100. F120. ;
Position, drill hole 1, then return to point R.
Y-550. ;
Position, drill hole 2, then return to point R.
Y-750. ;
Position, drill hole 3, then return to point R.
X1000. ;
Position, drill hole 4, then return to point R.
Y-550. ;
Position, drill hole 5, then return to point R.
G98 Y-750. ;
Position, drill hole 6, then return to the initial level.
G80 G28 G91 X0 Y0 Z0 ;
Return to the reference position
M5 ;
Cause the spindle to stop rotating.
- 46 -
5.FUNCTIONS TO SIMPLIFY
B-64304EN-2/01
PROGRAMMING
PROGRAMMING
5.1.5
Drilling Cycle Counter Boring Cycle (G82)
This cycle is used for normal drilling.
Cutting feed is performed to the bottom of the hole. At the bottom, a
dwell is performed, then the tool is retracted in rapid traverse.
This cycle is used to drill holes more accurately with respect to depth.
Format
G82 X_ Y_ Z_ R_ P_ F_ K_ ;
X_ Y_ : Hole position data
Z_
: The distance from point R to the bottom of the hole
R_
: The distance from the initial level to point R level
P_
: Dwell time at the bottom of a hole
F_
: Cutting feed rate
K_
: Number of repeats (if required)
G82 (G98)
G82 (G99)
Initial level
Point R level
Point R
Point R
Point Z
Point Z
P
P
Explanation
- Operations
After positioning along the X- and Y-axes, rapid traverse is performed
to point R.
Drilling is then performed from point R to point Z.
When the bottom of the hole has been reached, a dwell is performed.
The tool is then retracted in rapid traverse.
- Spindle rotation
Before specifying G82, use an auxiliary function (M code) to rotate
the spindle.
- Auxiliary function
When the G82 command and an M code are specified in the same
block, the M code is executed at the time of the first positioning
operation. When K is used to specify the number of repeats, the M
code is executed for the first hole only; for the second and subsequent
holes, the M code is not executed.
- 47 -
5. FUNCTIONS TO SIMPLIFY
PROGRAMMING
PROGRAMMING
B-64304EN-2/01
- Tool length compensation
When a tool length compensation (G43, G44, or G49) is specified in
the canned cycle for drilling, the offset is applied after the time of
positioning to point R.
Limitation
- Axis switching
Before the drilling axis can be changed, the canned cycle for drilling
must be canceled.
- Drilling
In a block that does not contain X, Y, Z, R, or any other axes, drilling
is not performed.
- P
Specify P in blocks that perform drilling. If it is specified in a block
that does not perform drilling, it cannot be stored as modal data.
- Cancel
Do not specify a G code of the 01 group (G00 to G03) and G82 in a
single block. Otherwise, G82 will be canceled.
- Tool offset
In the canned cycle mode for drilling, tool offsets are ignored.
Example
M3 S2000 ;
Cause the spindle to start rotating.
G90 G99 G82 X300. Y-250. Z-150. R-100. P1000 F120. ;
Position, drill hole
1, and dwell for 1 s at the
bottom of the hole, then return to point R.
Y-550. ;
Position, drill hole 2, then return to point R.
Y-750. ;
Position, drill hole 3, then return to point R.
X1000. ;
Position, drill hole 4, then return to point R.
Y-550. ;
Position, drill hole 5, then return to point R.
G98 Y-750. ;
Position, drill hole 6, then return to the initial level.
G80 G28 G91 X0 Y0 Z0
; Return to the reference position
M5 ;
Cause the spindle to stop rotating.
- 48 -
5.FUNCTIONS TO SIMPLIFY
B-64304EN-2/01
PROGRAMMING
PROGRAMMING
5.1.6
Peck Drilling Cycle (G83)
This cycle performs peck drilling.
It performs intermittent cutting feed to the bottom of a hole while
removing shavings from the hole.
Format
G83 X_ Y_ Z_ R_ Q_ F_ K_ ;
X_ Y_ : Hole position data
Z_
: The distance from point R to the bottom of the hole
R_
: The distance from the initial level to point R level
Q_
: Depth of cut for each cutting feed
F_
: Cutting feedrate
K_
: Number of repeats (if required)
G83 (G98)
G83 (G99)
Initial level
Point R level
Point R
Point R
q
q
d
d
q
q
d
d
q
q
Point Z
Point Z
Explanation
- Operations
Q represents the depth of cut for each cutting feed. It must always be
specified as an incremental value.
In the second and subsequent cutting feeds, rapid traverse is
performed up to a d point just before where the last drilling ended, and
cutting feed is performed again. d is set in parameter (No.5115).
Be sure to specify a positive value in Q. Negative values are
ignored.
- Spindle rotation
Before specifying G83, use an auxiliary function (M code) to rotate
the spindle.
- Auxiliary function
When the G83 command and an M code are specified in the same
block, the M code is executed at the time of the first positioning
operation. When K is used to specify the number of repeats, the M
code is executed for the first hole only; for the second and subsequent
holes, the M code is not executed.
- 49 -
5. FUNCTIONS TO SIMPLIFY
PROGRAMMING
PROGRAMMING
B-64304EN-2/01
- Tool length compensation
When a tool length compensation (G43, G44, or G49) is specified in
the canned cycle for drilling, the offset is applied after the time of
positioning to point R.
Limitation
- Axis switching
Before the drilling axis can be changed, the canned cycle for drilling
must be canceled.
- Drilling
In a block that does not contain X, Y, Z, R, or any other axes, drilling
is not performed.
- Q
Specify Q in blocks that perform drilling. If they are specified in a
block that does not perform drilling, they cannot be stored as modal
data.
- Cancel
Do not specify a G code of the 01 group (G00 to G03) and G83 in a
single block. Otherwise, G83 will be canceled.
- Tool offset
In the canned cycle mode for drilling, tool offsets are ignored.
Example
M3 S2000 ;
Cause the spindle to start rotating.
G90 G99 G83 X300. Y-250. Z-150. R-100. Q15. F120. ;
Position, drill hole 1, then return to point R.
Y-550. ;
Position, drill hole 2, then return to point R.
Y-750. ;
Position, drill hole 3, then return to point R.
X1000. ;
Position, drill hole 4, then return to point R.
Y-550. ;
Position, drill hole 5, then return to point R.
G98 Y-750. ;
Position, drill hole 6, then return to the initial level.
G80 G28 G91 X0 Y0 Z0 ;
Return to the reference position
M5 ;
Cause the spindle to stop rotating.
- 50 -
5.FUNCTIONS TO SIMPLIFY
B-64304EN-2/01
PROGRAMMING
PROGRAMMING
5.1.7
Small-Hole Peck Drilling Cycle (G83)
An arbor with the overload torque detection function is used to retract
the tool when the overload torque detection signal (skip signal) is
detected during drilling. Drilling is resumed after the spindle speed
and cutting feedrate are changed. These steps are repeated in this peck
drilling cycle.
The mode for the small-hole peck drilling cycle is selected when the
M code in parameter 5163 is specified. The cycle can be started by
specifying G83 in this mode. This mode is canceled when G80 is
specified or when a reset occurs.
NOTE
When using the small-hole peck drilling cycle, set
bit 4 (SPK) of parameter No. 8132 to "1".
- 51 -
5. FUNCTIONS TO SIMPLIFY
PROGRAMMING
PROGRAMMING
B-64304EN-2/01
Format
G83 X_ Y_ Z_ R_ Q_ F_ I_ K_ P_ ;
X_ Y_ : Hole position data
Z_
: Distance from point R to the bottom of the hole
R_
: Distance from the initial level to point R
Q_
: Depth of each cut
F_
: Cutting feedrate
I_
: Forward or backward traveling speed (same format
as F above)
(If this is omitted, the values in parameters
No.5172 and No.5173 are assumed as defaults.)
K_
: Number of times the operation is repeated (if
required)
P_
: Dwell time at the bottom of the hole
(If this is omitted, P0 is assumed as the default.)
G83 (G98)
G83 (G99)
Initial level
Point R
Point R
Point R level
q
q
∆
∆
∆
∆
Overload torque
Overload torque
Point Z
Point Z
Dwell
Dwell
∆: Initial clearance when the tool is retracted to point R and the clearance from the
bottom of the hole in the second or subsequent drilling (parameter 5174)
q: Depth of each cut
Path along which the tool travels at the rapid traverse rate
Path along which the tool travels at the programmed cutting
feedrate
Path along which the tool travels at the forward or backward rate during the
(
) cycle specified with parameters
- 52 -
5.FUNCTIONS TO SIMPLIFY
B-64304EN-2/01
PROGRAMMING
PROGRAMMING
Explanations
- Component operations of the cycle
* X- and Y-axis positioning
* Positioning at point R along the Z-axis
* Cutting along the Z-axis (first time, depth of cut Q, incremental)
Retracting
(bottom of hole → minimum clearance ¨, incremental)
Retraction
Repeated until
(bottom of hole +∆ → to point R, absolute)
point Z is reached
Forwarding
(point R → to point with hole bottom + clearance ¨, absolute)
Cutting
(second and subsequent times, cut of depth Q + ¨, incremental)
* Dwell
* Return to point R along the Z-axis (or initial point) = end of
cycle
Acceleration/deceleration during advancing and retraction is
controlled according to the cutting feed acceleration/deceleration time
constant.
When retraction is performed, the position is checked at point R.
- Specifying an M code
When the M code in parameter 5163 is specified, the system enters the
mode for the small-hole peck drilling cycle.
This M code does not wait for FIN. Care must be taken when this M
code is specified with another M code in the same block.
(Example) M03 M
; → Waits for FIN.
M M03 ; → Does not wait for FIN.
- Specifying a G code
When G83 is specified in the mode for the small-hole peck drilling
cycle, the cycle is started.
This continuous-state G code remains unchanged until another canned
cycle is specified or until the G code for canceling the canned cycle is
specified. This eliminates the need for specifying drilling data in each
block when identical drilling is repeated.
- Signal indicating that the cycle is in progress
In this cycle, the signal indicating that the small-hole peck drilling
cycle is in progress is output after the tool is positioned at the hole
position along the axes not used for drilling. Signal output continues
during positioning to point R along the drilling axis and terminates
upon a return to point R or the initial level. For details, refer to the
manual of the machine tool builder.
- 53 -
5. FUNCTIONS TO SIMPLIFY
PROGRAMMING
PROGRAMMING
B-64304EN-2/01
- Overload torque detection signal
A skip signal is used as the overload torque detection signal. The skip
signal is effective while the tool is advancing or drilling and the tool
tip is between points R and Z. (The signal causes a retraction). For
details, refer to the manual of the machine tool builder.
NOTE
When receiving overload torque detect signal while the
tool is advancing, the tool will be retracted (clearance ∆
and to the point R), then advanced to the same target
point as previous advancing.
- Changing the drilling conditions
In a single G83 cycle, drilling conditions are changed for each drilling
operation
(advance
→ drilling
→ retraction). Bits
1 and
2 of
parameter OLS, NOL No. 5160 can be specified to suppress the
change in drilling conditions.
1
Changing the cutting feedrate
The cutting feedrate programmed with the F code is changed for
each of the second and subsequent drilling operations. In
parameters No.5166 and No.5167, specify the respective rates of
change applied when the skip signal is detected and when it is
not detected in the previous drilling operation.
Cutting feedrate = F × α
<First drilling> α=1.0
<Second or subsequent drilling> α=α×β÷100, where β is the rate
of change for each drilling operation
When the skip signal is detected during the previous drilling
operation: β=b1% (parameter No.5166)
When the skip signal is not detected during the previous drilling
operation: β=b2% (parameter No.5167)
If the rate of change in cutting feedrate becomes smaller than the
rate specified in parameter
5168, the cutting feedrate is not
changed.
The cutting feedrate can be increased up to the maximum cutting
feedrate.
2
Changing the spindle speed
The spindle speed programmed with the S code is changed for
each of the second and subsequent advances. In parameters 5164
and 5165, specify the rates of change applied when the skip
signal is detected and when it is not detected in the previous
drilling operation.
Spindle speed = S × γ
- 54 -
5.FUNCTIONS TO SIMPLIFY
B-64304EN-2/01
PROGRAMMING
PROGRAMMING
<First drilling> γ=1.0
<Second or subsequent drilling> γ=γ×δ÷100, where δ is the rate
of change for each drilling operation
When the skip signal is detected during the previous drilling
operation: δ=d1% (parameter No.5164)
When the skip signal is not detected during the previous drilling
operation: δ=d2% (parameter No.5165)
When the cutting feedrate reaches the minimum rate, the spindle
speed is not changed. The spindle speed can be increased up to a
value corresponding to the maximum value of S analog data.
- Advance and retraction
Advancing and retraction of the tool are not executed in the same
manner as rapid-traverse positioning. Like cutting feed, the two
operations are carried out as interpolated operations. Note that the tool
life management function excludes advancing and retraction from the
calculation of the tool life.
- Specifying address I
The forward or backward traveling speed can be specified with
address I in the same format as address F, as shown below:
G83 I1000 ; (without decimal point)
G83 I1000. ; (with decimal point)
Both commands indicate a speed of 1000 mm/min.
Address I specified with G83 in the continuous-state mode continues
to be valid until G80 is specified or until a reset occurs.
NOTE
If address I is not specified and parameter No.5172 (for
backward) or No.5173 (for forward) is set to 0, the
forward or backward travel speed is same as the cutting
feedrate specified by F.
- Functions that can be specified
In this canned cycle mode, the following functions can be specified:
•
Hole position on the X-axis, Y-axis, and additional axis
•
Operation and branch by custom macro
•
Subprogram (hole position group, etc.) calling
•
Switching between absolute and incremental modes
•
Coordinate system rotation
•
Scaling (This command will not affect depth of cut Q or small
clearance ∆.)
•
Dry run
•
Feed hold
- Single block
When single-block operation is enabled, drilling is stopped after each
retraction. Also, a single block stop is performed by setting parameter
SBC (No.5105 bit 0)
- 55 -
5. FUNCTIONS TO SIMPLIFY
PROGRAMMING
PROGRAMMING
B-64304EN-2/01
- Feedrate override
The feedrate override function works during cutting, retraction, and
advancing in the cycle.
- Custom macro interface
The number of retractions made during cutting and the number of
retractions made in response to the overload signal received during
cutting can be output to custom macro common variables (#100 to
#149) specified in parameters No.5170 and No.5171. Parameters
No.5170 and No.5171 can specify variable numbers within the range
of #100 to #149.
Parameter No.5170: Specifies the number of the common variable to
which the number of retractions made during
cutting is output.
Parameter No.5171: Specifies the number of the common variable to
which the number of retractions made in
response to the overload signal received during
cutting is output.
NOTE
The numbers of retraction output to common
variables are cleared by G83 while small-hole peck
drilling cycle mode.
Limitation
- Subprogram call
In the canned cycle mode, specify the subprogram call command
M98P_ in an independent block.
Example
M03 S_ ; Cause the spindle to start rotating.
M
;
Specifies the small-hole peck drilling cycle mode.
G83 X_ Y_ Z_ R_ Q_ F_ I_ K_ P_ ;
Specifies the small-hole peck drilling cycle.
X_ Y_ ; Drills at another position.
:
:
G80 ;
Cancels the small-hole peck drilling cycle mode.
- 56 -
5.FUNCTIONS TO SIMPLIFY
B-64304EN-2/01
PROGRAMMING
PROGRAMMING
5.1.8
Tapping Cycle (G84)
This cycle performs tapping.
In this tapping cycle, when the bottom of the hole has been reached,
the spindle is rotated in the reverse direction.
Format
G84 X_ Y_ Z_ R_ P_ Q_ F_ K_ ;
X_ Y_ : Hole position data
Z_
: The distance from point R to the bottom of the hole
R_
: The distance from the initial level to point R level
P_
: Dwell time
Q_
: Depth of cut for each cutting feed (bit 6 (PCT) of
parameter No. 5104 = "1")
F_
: Cutting feedrate
K_
: Number of repents (if required)
G84 (G98)
G84 (G99)
Initial level
Spindle
Spindle
CW
CW
P
Point R
P
Point R
Point R level
P
Point Z
P
Point Z
Spindle CCW
Spindle CCW
Explanation
- Operations
Tapping is performed by rotating the spindle clockwise. When the
bottom of the hole has been reached, the spindle is rotated in the
reverse direction for retraction. This operation creates threads.
CAUTION
Feedrate overrides are ignored during tapping. A
feed hold does not stop the machine until the return
operation is completed.
- 57 -
5. FUNCTIONS TO SIMPLIFY
PROGRAMMING
PROGRAMMING
B-64304EN-2/01
- Spindle rotation
Before specifying G84, use an auxiliary function (M code) to rotate
the spindle.
If drilling is continuously performed with a small value specified for
the distance between the hole position and point R level or between
the initial level and point R level, the normal spindle speed may not be
reached at the start of hole cutting operation. In this case, insert a
dwell before each drilling operation with G04 to delay the operation,
without specifying the number of repeats for K. For some machines,
the above note may not be considered. Refer to the manual provided
by the machine tool builder.
- Q command
See “Left-Handed Tapping Cycle (G74)” above.
- Auxiliary function
When the G84 command and an M code are specified in the same
block, the M code is executed at the time of the first positioning
operation. When the K is used to specify number of repeats, the M
code is executed for the first hole only; for the second and subsequent
holes, the M code is not executed.
- Tool length compensation
When a tool length compensation (G43, G44, or G49) is specified in
the canned cycle for drilling, the offset is applied after the time of
positioning to point R.
Limitation
- Axis switching
Before the drilling axis can be changed, the canned cycle for drilling
must be canceled.
- Drilling
In a block that does not contain X, Y, Z, R, or any other axes, drilling
is not performed.
- P
Specify P in blocks that perform drilling. If it is specified in a block
that does not perform drilling, it cannot be stored as modal data.
- Cancel
Do not specify a G code of the 01 group (G00 to G03) and G84 in a
single block. Otherwise, G84 will be canceled.
- 58 -
5.FUNCTIONS TO SIMPLIFY
B-64304EN-2/01
PROGRAMMING
PROGRAMMING
Example
M3 S100 ;
Cause the spindle to start rotating.
G90 G99 G84 X300. Y-250. Z-150. R-120. P300 F120. ;
Position, drill hole 1, then return to point R.
Y-550. ;
Position, drill hole 2, then return to point R.
Y-750. ;
Position, drill hole 3, then return to point R.
X1000. ;
Position, drill hole 4, then return to point R.
Y-550. ;
Position, drill hole 5, then return to point R.
G98 Y-750. ;
Position, drill hole
6, then return to the initial
level.
G80 G28 G91 X0 Y0 Z0
;
Return to the reference position
M5 ;
Cause the spindle to stop rotating.
- 59 -
5. FUNCTIONS TO SIMPLIFY
PROGRAMMING
PROGRAMMING
B-64304EN-2/01
5.1.9
Boring Cycle (G85)
This cycle is used to bore a hole.
Format
G85 X_ Y_ Z_ R_ F_ K_ ;
X_ Y_ : Hole position data
Z_
: The distance from point R to the bottom of the hole
R_
: The distance from the initial level to point R level
F_
: Cutting feed rate
K_
: Number of repeats (if required)
G85 (G98)
G85 (G99)
Initial level
Point R
Point R
Point R level
Point Z
Point Z
Explanation
- Operations
After positioning along the X- and Y- axes, rapid traverse is
performed to point R.
Drilling is performed from point R to point Z.
When point Z has been reached, cutting feed is performed to return to
point R.
- Spindle rotation
Before specifying G85, use an auxiliary function (M code) to rotate
the spindle.
- Auxiliary function
When the G85 command and an M code are specified in the same
block, the M code is executed at the time of the first positioning
operation. When K is used to specify the number of repeats, the M
code is executed for the first hole only; for the second and subsequent
holes, the M code is not executed.
- Tool length compensation
When a tool length compensation (G43, G44, or G49) is specified in
the canned cycle for drilling, the offset is applied after the time of
positioning to point R.
- 60 -
5.FUNCTIONS TO SIMPLIFY
B-64304EN-2/01
PROGRAMMING
PROGRAMMING
Limitation
- Axis switching
Before the drilling axis can be changed, the canned cycle for drilling
must be canceled.
- Drilling
In a block that does not contain X, Y, Z, R, or any other axes, drilling
is not performed.
- Cancel
Do not specify a G code of the 01 group (G00 to G03) and G85 in a
single block. Otherwise, G85 will be canceled.
- Tool offset
In the canned cycle mode for drilling, tool offsets are ignored.
Example
M3 S100 ;
Cause the spindle to start rotating.
G90 G99 G85 X300. Y-250. Z-150. R-120. F120. ;
Position, drill hole 1, then return to point R.
Y-550. ;
Position, drill hole 2, then return to point R.
Y-750. ;
Position, drill hole 3, then return to point R.
X1000. ;
Position, drill hole 4, then return to point R.
Y-550. ;
Position, drill hole 5, then return to point R.
G98 Y-750. ;
Position, drill hole
6, then return to the
initial level.
G80 G28 G91 X0 Y0 Z0
;Return to the reference position
M5 ;
Cause the spindle to stop rotating.
- 61 -
5. FUNCTIONS TO SIMPLIFY
PROGRAMMING
PROGRAMMING
B-64304EN-2/01
5.1.10
Boring Cycle (G86)
This cycle is used to bore a hole.
Format
G86 X_ Y_ Z_ R_ F_ K_ ;
X_ Y_ : Hole position data
Z_
: The distance from point R to the bottom of the hole
R_
: The distance from the initial level to point R level
F_
: Cutting feed rate
K_
: Number of repeats (if required)
G86 (G98)
G86 (G99)
Spindle CW
Initial level
Spindle CW
Point R
Point R
Point R level
Point Z
Point Z
Spindle stop
Spindle stop
Explanation
- Operations
After positioning along the X- and Y-axes, rapid traverse is performed
to point R.
Drilling is performed from point R to point Z.
When the spindle is stopped at the bottom of the hole, the tool is
retracted in rapid traverse.
- Spindle rotation
Before specifying G86, use an auxiliary function (M code) to rotate
the spindle.
If drilling is continuously performed with a small value specified for
the distance between the hole position and point R level or between
the initial level and point R level, the normal spindle speed may not be
reached at the start of hole cutting operation. In this case, insert a
dwell before each drilling operation with G04 to delay the operation,
without specifying the number of repeats for K. For some machines,
the above note may not be considered. Refer to the manual provided
by the machine tool builder.
- 62 -
5.FUNCTIONS TO SIMPLIFY
B-64304EN-2/01
PROGRAMMING
PROGRAMMING
- Auxiliary function
When the G86 command and an M code are specified in the same
block, the M code is executed at the time of the first positioning
operation. When K is used to specify the number of repeats, the M
code is executed for the first hole only; for the second and subsequent
holes, the M code is not executed.
- Tool length compensation
When a tool length compensation (G43, G44, or G49) is specified in
the canned cycle for drilling, the offset is applied after the time of
positioning to point R.
Limitation
- Axis switching
Before the drilling axis can be changed, the canned cycle for drilling
must be canceled.
- Drilling
In a block that does not contain X, Y, Z, R, or any other axes, drilling
is not performed.
- Cancel
Do not specify a G code of the 01 group (G00 to G03) and G86 in a
single block. Otherwise, G86 will be canceled.
- Tool offset
In the canned cycle mode for drilling, tool offsets are ignored.
Example
M3 S2000 ;
Cause the spindle to start rotating.
G90 G99 G86 X300. Y-250. Z-150. R-100. F120. ;
Position, drill hole 1, then return to point R.
Y-550. ;
Position, drill hole 2, then return to point R.
Y-750. ;
Position, drill hole 3, then return to point R.
X1000. ;
Position, drill hole 4, then return to point R.
Y-550. ;
Position, drill hole 5, then return to point R.
G98 Y-750. ;
Position, drill hole
6, then return to the initial
level.
G80 G28 G91 X0 Y0 Z0
;
Return to the reference position
M5 ;
Cause the spindle to stop rotating.
- 63 -
5. FUNCTIONS TO SIMPLIFY
PROGRAMMING
PROGRAMMING
B-64304EN-2/01
5.1.11 Back Boring Cycle (G87)
This cycle performs accurate boring.
Format
G87 X_ Y_ Z_ R_ Q_ P_ F_ K_ ;
X_ Y_ : Hole position data
Z_
: The distance from point R to the bottom of the hole
R_
: The distance from the initial level to point R
Q_
: Shift amount at the bottom of a hole
P_
: Dwell time at the bottom of a hole
F_
: Cutting feed rate
K_
: Number of repeats (if required)
G87 (G98)
G87 (G99)
Spindle orientation
q
Tool
OSS
Initial
level
Spindle CW
Not used
OSS
Point Z
P
Spindle CW
Point R
Shift amount q
Explanation
After positioning along the X- and Y-axes, the spindle is stopped at
the fixed rotation position. The tool is moved in the direction
opposite to the tool nose, positioning (rapid traverse) is performed to
the bottom of the hole (point R).
The tool is then shifted in the direction of the tool nose and the spindle
is rotated clockwise. Boring is performed in the positive direction
along the Z-axis until point Z is reached.
At point Z, the spindle is stopped at the fixed rotation position again,
the tool is shifted in the direction opposite to the tool nose, then the
tool is returned to the initial level. The tool is then shifted in the
direction of the tool nose and the spindle is rotated clockwise to
proceed to the next block operation.
- Spindle rotation
Before specifying G87, use an auxiliary function (M code) to rotate
the spindle.
If drilling is continuously performed with a small value specified for
the distance between the hole position and point R level or between
the initial level and point R level, the normal spindle speed may not be
reached at the start of hole cutting operation. In this case, insert a
dwell before each drilling operation with G04 to delay the operation,
without specifying the number of repeats for K. For some machines,
the above note may not be considered. Refer to the manual provided
by the machine tool builder.
- 64 -
5.FUNCTIONS TO SIMPLIFY
B-64304EN-2/01
PROGRAMMING
PROGRAMMING
- Auxiliary function
When the G87 command and an M code are specified in the same
block, the M code is executed at the time of the first positioning
operation. When K is used to specify the number of repeats, the M
code is executed for the first hole only; for the second and subsequent
holes, the M code is not executed.
- Tool length compensation
When a tool length compensation (G43, G44, or G49) is specified in
the canned cycle for drilling, the offset is applied after the time of
positioning to point R.
Limitation
- Axis switching
Before the drilling axis can be changed, the canned cycle for drilling
must be canceled.
- Drilling
In a block that does not contain X, Y, Z, R, or any additional axes,
drilling is not performed.
- P/Q
Be sure to specify a positive value in Q. If Q is specified with a
negative value, the sign is ignored. Set the direction of shift in the
parameter (No. 5148).
Specify P and Q in a block that performs drilling. If they are
specified in a block that does not perform drilling, they are not stored
as modal data.
CAUTION
Q (shift at the bottom of a hole) is a modal value
retained in canned cycles for drilling. It must be
specified carefully because it is also used as the
depth of cut for G73 and G83.
- Cancel
Do not specify a G code of the 01 group (G00 to G03) and G87 in a
single block. Otherwise, G87 will be canceled.
- Tool offset
In the canned cycle mode for drilling, tool offsets are ignored.
- 65 -
5. FUNCTIONS TO SIMPLIFY
PROGRAMMING
PROGRAMMING
B-64304EN-2/01
Example
M3 S500 ;
Cause the spindle to start rotating.
G90 G87 X300. Y-250.
Position, bore hole 1.
Z-150. R-120. Q5.
Orient at the initial level, then shift by 5 mm.
P1000 F120. ;
Stop at point Z for 1 s.
Y-550. ;
Position, drill hole 2.
Y-750. ;
Position, drill hole 3.
X1000. ;
Position, drill hole 4.
Y-550. ;
Position, drill hole 5.
Y-750. ;
Position, drill hole 6
G80 G28 G91 X0 Y0 Z0 ;
Return to the reference position
M5 ;
Cause the spindle to stop rotating.
- 66 -
5.FUNCTIONS TO SIMPLIFY
B-64304EN-2/01
PROGRAMMING
PROGRAMMING
5.1.12
Boring Cycle (G88)
This cycle is used to bore a hole.
Format
G88 X_ Y_ Z_ R_ P_ F_ K_ ;
X_ Y_ : Hole position data
Z_
: The distance from point R to the bottom of the hole
R_
: The distance from the initial level to point R level
P_
: Dwell time at the bottom of a hole
F_
: Cutting feed rate
K_
: Number of repeats (if required)
G88 (G98)
G88 (G99)
Spindle CW
Initial level
Spindle CW
Point R
Point R
Point R level
Point Z
Point Z
P
P
Spindle stop
Spindle stop
after dwell
after dwell
Explanation
- Operations
After positioning along the X- and Y-axes, rapid traverse is performed
to point R. Boring is performed from point R to point Z.
When boring is completed, a dwell is performed at the bottom of the
hole, then the spindle is stopped and enters the hold state. At this
time, you can switch to the manual mode and move the tool manually.
Any manual operations are available; it is desirable to finally retract
the tool from the hole for safety, though.
At the restart of machining in the DNC operation or memory mode,
the tool returns to the initial level or point R level according to G98 or
G99 and the spindle rotates clockwise. Then, operation is restarted
according to the programmed commands in the next block.
- Spindle rotation
Before specifying G88, use an auxiliary function (M code) to rotate
the spindle.
- 67 -
5. FUNCTIONS TO SIMPLIFY
PROGRAMMING
PROGRAMMING
B-64304EN-2/01
- Auxiliary function
When the G88 command and an M code are specified in the same
block, the M code is executed at the time of the first positioning
operation. When K is used to specify the number of repeats, the M
code is executed for the first hole only; for the second and subsequent
holes, the M code is not executed.
- Tool length compensation
When a tool length compensation (G43, G44, or G49) is specified in
the canned cycle for drilling, the offset is applied after the time of
positioning to point R.
Limitation
- Axis switching
Before the drilling axis can be changed, the canned cycle for drilling
must be canceled.
- Drilling
In a block that does not contain X, Y, Z, R, or any other axes, drilling
is not performed.
- P
Specify P in blocks that perform drilling. If it is specified in a block
that does not perform drilling, it cannot be stored as modal data.
- Cancel
Do not specify a G code of the 01 group (G00 to G03) and G88 in a
single block. Otherwise, G88 will be canceled.
- Tool offset
In the canned cycle mode for drilling, tool offsets are ignored.
Example
M3 S2000 ;
Cause the spindle to start rotating.
G90 G99 G88 X300. Y-250. Z-150. R-100. P1000 F120. ;
Position, drill hole 1, return to point R then stop
at the bottom of the hole for 1 s.
Y-550. ;
Position, drill hole 2, then return to point R.
Y-750. ;
Position, drill hole 3, then return to point R.
X1000. ;
Position, drill hole 4, then return to point R.
Y-550. ;
Position, drill hole 5, then return to point R.
G98 Y-750. ;
Position, drill hole
6, then return to the initial
level.
G80 G28 G91 X0 Y0 Z0
;
Return to the reference position
M5 ;
Cause the spindle to stop rotating.
- 68 -
5.FUNCTIONS TO SIMPLIFY
B-64304EN-2/01
PROGRAMMING
PROGRAMMING
5.1.13 Boring Cycle (G89)
This cycle is used to bore a hole.
Format
G89 X_ Y_ Z_ R_ P_ F_ K_ ;
X_ Y_ : Hole position data
Z_
: The distance from point R to the bottom of the hole
R_
: The distance from the initial level to point R level
P_
: Dwell time at the bottom of a hole
F_
: Cutting feed rate
K_
: Number of repeats (if required)
G89 (G98)
G89 (G99)
Initial level
Point R
Point R
Point R level
Point Z
Point Z
P
P
Explanation
- Operations
This cycle is almost the same as G85. The difference is that this
cycle performs a dwell at the bottom of the hole.
- Spindle rotation
Before specifying G89, use an auxiliary function (M code) to rotate
the spindle.
- Auxiliary function
When the G89 command and an M code are specified in the same
block, the M code is executed at the time of the first positioning
operation. When K is used to specify the number of repeats, the M
code is executed for the first hole only; for the second and subsequent
holes, the M code is not executed.
- Tool length compensation
When a tool length compensation (G43, G44, or G49) is specified in
the canned cycle for drilling, the offset is applied after the time of
positioning to point R.
- 69 -
5. FUNCTIONS TO SIMPLIFY
PROGRAMMING
PROGRAMMING
B-64304EN-2/01
Limitation
- Axis switching
Before the drilling axis can be changed, the canned cycle for drilling
must be canceled.
- Drilling
In a block that does not contain X, Y, Z, R, or any other axes, drilling
is not performed.
- P
Specify P in blocks that perform drilling. If it is specified in a block
that does not perform drilling, it cannot be stored as modal data.
- Cancel
Do not specify a G code of the 01 group (G00 to G03) and G89 in a
single block. Otherwise, G89 will be canceled.
- Tool offset
In the canned cycle mode for drilling, tool offsets are ignored.
Example
M3 S100 ;
Cause the spindle to start rotating.
G90 G99 G89 X300. Y-250. Z-150. R-120. P1000 F120. ;
Position, drill hole 1, return to point R then stop
at the bottom of the hole for 1 s.
Y-550. ;
Position, drill hole 2, then return to point R.
Y-750. ;
Position, drill hole 3, then return to point R.
X1000. ;
Position, drill hole 4, then return to point R.
Y-550. ;
Position, drill hole 5, then return to point R.
G98 Y-750. ;
Position, drill hole
6, then return to the initial
level.
G80 G28 G91 X0 Y0 Z0
;
Return to the reference position
M5 ;
Cause the spindle to stop rotating.
- 70 -
5.FUNCTIONS TO SIMPLIFY
B-64304EN-2/01
PROGRAMMING
PROGRAMMING
5.1.14 Canned Cycle Cancel for Drilling (G80)
G80 cancels canned cycles for drilling.
Format
G80 ;
Explanation
All canned cycles for drilling are canceled to perform normal
operation. Point R and point Z are cleared.
Other drilling data is also canceled (cleared).
Example
M3 S100 ;
Cause the spindle to start rotating.
G90 G99 G88 X300. Y-250. Z-150. R-120. F120. ;
Position, drill hole 1, then return to point R.
Y-550. ;
Position, drill hole 2, then return to point R.
Y-750. ;
Position, drill hole 3, then return to point R.
X1000. ;
Position, drill hole 4, then return to point R.
Y-550. ;
Position, drill hole 5, then return to point R.
G98 Y-750. ;
Position, drill hole
6, then return to the initial
level.
G80 G28 G91 X0 Y0 Z0
;
Return to the reference position, canned cycle
cancel
M5 ;
Cause the spindle to stop rotating.
- 71 -
5. FUNCTIONS TO SIMPLIFY
PROGRAMMING
PROGRAMMING
B-64304EN-2/01
5.1.15 Example for Using Canned Cycles for Drilling
Offset value +200.0 is set in offset No.11, +190.0 is set in offset No.15, and +150.0 is set in offset No.31
Program example
;
N001
G92 X0 Y0 Z0;
Coordinate setting at reference position
N002
G90 G00 Z250.0 T11 M6;
Tool change
N003
G43 Z0 H11;
Initial level, tool length compensation
N004
S30 M3;
Spindle start
N005
G99 G81 X400.0 Y-350.0 Z-153.0 R-97.0 F120;
Positioning, then #1 drilling
N006
Y-550.0;
Positioning, then #2 drilling and point R level return
N007
G98 Y-750.0;
Positioning, then #3 drilling and initial level return
N008
G99 X1200.0;
Positioning, then #4 drilling and point R level return
N009
Y-550.0;
Positioning, then #5 drilling and point R level return
N010
G98 Y-350.0;
Positioning, then #6 drilling and initial level return
N011
G00 X0 Y0 M5;
Reference position return, spindle stop
N012
G49 Z250.0 T15 M6;
Tool length compensation cancel, tool change
N013
G43 Z0 H15;
Initial level, tool length compensation
N014
S20 M3;
Spindle start
N015
G99 G82 X550.0 Y-450.0 Z-130.0 R-97.0 P300 F70;
Positioning, then #7 drilling, point R level return
N016
G98 Y-650.0;
Positioning, then #8 drilling, initial level return
N017
G99 X1050.0;
Positioning, then #9 drilling, point R level return
N018
G98 Y-450.0;
Positioning, then #10 drilling, initial level return
N019
G00 X0 Y0 M5;
Reference position return, spindle stop
N020
G49 Z250.0 T31 M6;
Tool length compensation cancel, tool change
N021
G43 Z0 H31;
Initial level, tool length compensation
N022
S10 M3;
Spindle start
N023
G85 G99 X800.0 Y-350.0 Z-153.0 R47.0 F50;
Positioning, then #11 drilling, point R level return
N024
G91 Y-200.0 K2;
Positioning, then #12, 13 drilling, point R level return
N025
G28 X0 Y0 M5;
Reference position return, spindle stop
N026
G49 Z0;
Tool length compensation cancel
N027
M0;
Program stop
- 72 -
5.FUNCTIONS TO SIMPLIFY
B-64304EN-2/01
PROGRAMMING
PROGRAMMING
Program using tool length offset and canned cycles
Reference position
350
#1
#11
#6
100
#7
200
#10
100
#2
#12
#5
100
#8
#9
Y
200
100
#3
#13
#4
X
400
150
250
250
150
#1 to 6
Drilling of a 10 mm diameter hole
#7 to 10
Drilling of a 20 mm diameter hole
#11 to 13
Boring of a 95 mm diameter hole (depth 50 mm)
Z
Retract position
250
Initial level
X
50
50
30
20
T 11
T 15
T 31
200
190
150
Fig. 5.1.15 (a) Example for using canned cycles for drilling
- 73 -
5. FUNCTIONS TO SIMPLIFY
PROGRAMMING
PROGRAMMING
B-64304EN-2/01
5.2
RIGID TAPPING
The tapping cycle (G84) and left-handed tapping cycle (G74) may be
performed in standard mode or rigid tapping mode.
In standard mode, the spindle is rotated and stopped along with a
movement along the tapping axis using auxiliary functions M03
(rotating the spindle clockwise), M04
(rotating the spindle
counterclockwise), and M05
(stopping the spindle) to perform
tapping.
In rigid mode, tapping is performed by controlling the spindle motor
as if it were a servo motor and by interpolating between the tapping
axis and spindle.
When tapping is performed in rigid mode, the spindle rotates one turn
every time a certain feed (thread lead) which takes place along the
tapping axis. This operation does not vary even during acceleration
or deceleration.
Rigid mode eliminates the need to use a floating tap required in the
standard tapping mode, thus allowing faster and more precise tapping.
- 74 -
5.FUNCTIONS TO SIMPLIFY
B-64304EN-2/01
PROGRAMMING
PROGRAMMING
5.2.1
Rigid Tapping (G84)
When the spindle motor is controlled in rigid mode as if it were a
servo motor, a tapping cycle can be speed up.
Format
G84 X_ Y_ Z_ R_ P_ F_ K_ ;
X_ Y_ : Hole position data
Z_
: The distance from point R to the bottom of the hole and the
position of the bottom of the hole
R_
: The distance from the initial level to point R level
P_
: Dwell time at the bottom of the hole and at point R when a return
is made
F_
: Cutting feedrate
K_
: Number of repeats (if required)
G84.2 X_ Y_ Z_ R_ P_ F_ L_ ;
(Series 10/11 format)
L_
: Number of repeats (if required)
G84 (G98)
G84 (G99)
Spindle stop
Spindle stop
Initial level
Operation 1
Operation 2
Operation 6
Spindle stop
Spindle CW
Spindle
P
Spindle CW
P
stop
Point R
Point R level
Point R
Point R level
Operation 3
Operation 5
Point Z
Point Z
P
P
Spindle stop
Spindle CCW
Spindle stop
Spindle CCW
Operation 4
Explanation
After positioning along the X- and Y-axes, rapid traverse is performed
to point R.
Tapping is performed from point R to point Z. When tapping is
completed, the spindle is stopped and a dwell is performed. The
spindle is then rotated in the reverse direction, the tool is retracted to
point R, then the spindle is stopped. Rapid traverse to initial level is
then performed.
While tapping is being performed, the feedrate override and spindle
override are assumed to be 100%. Feedrate override can be enabled
by setting, however.
- 75 -