Tapping a deep hole in rigid tapping mode may be difficult due to chips sticking to the tool or increased cutting resistance. In such cases, the peck rigid tapping cycle is useful.
In this cycle, cutting is performed several times until the bottom of the hole is reached. Two peck tapping cycles are available: High-speed peck tapping cycle and standard peck tapping cycle. These cycles are selected using the bit 5 (PCP) of parameter No. 5200.
Format
When rigid tapping is specified with G84 (G88) if bit 5 (PCP) of parameter No. 5200 = 0, high-speed peck rigid tapping is assumed.
Point R level
Point Z Point R
q
q
q
Mα
(1) (2) d
d
Spindle CCW Spindle stop M(α+1) P2
Spindle stop Spindle CCW
Spindle stop Spindle CW Spindle CW
Spindle stop P1 (3) Spindle stop
G84 or G88(G98 mode) G84 or G88(G99 mode)
G84 X(U)_ C(H)_Z(W)_ R_ P_ Q_ F_ K_ M_ ; or
G88 Z(W)_ C(H)_X(U)_ R_ P_ Q_ F_ K_ M_ ;
X_ C_ or Z_ C_ : Hole position data
Z_ or X_ : 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 the hole
Q_ : Depth of cut for each cutting feed F_ : The cutting feedrate
K_ : Number of repeats (when it is needed.) M_ : M code for C-axis clamp (when it is needed.)
- High-speed peck rigid tapping cycle In the first cutting from point R, perform cutting by depth "q" specified by address Q while rotating the spindle in the forward direction (operation <1>).
Then, perform returning by the amount specified by parameter No. 5213 while rotating the spindle in the reverse direction (operation <2>).
Then, perform tapping by (d+q) while rotating the spindle in the forward direction (operation <3>).
Repeat operations <2> and <3> until the bottom of the hole is reached.
The cutting speed and rigid tapping time constant are used for operations <1> and
<3>.
For operation <2> and travel from the bottom of the hole (point Z) to point R, rigid tapping extract override is enabled and the rigid tapping extract time constant is used.
d = Amount of return
Spindle stop
(3)
Point R level
P1 Spindle stop Spindle CW
Point R
Point Z
q
q
q
Mα
(1) (2) d
d Initial level
Spindle CCW Spindle stop M(α+1) P2
Spindle stop Spindle CCW
Spindle stop Spindle CW
When rigid tapping is specified with G84 (G88) if bit 5 (PCP) of parameter No. 5200 = 1, peck rigid tapping is assumed.
G84 or G88(G98 mode) G84 or G88(G99 mode)
G84 X(U)_ C(H)_Z(W)_ R_ P_ Q_ F_ K_ M_ ; or
G88 Z(W)_ C(H)_X(U)_ R_ P_ Q_ F_ K_ M_ ;
X_ C_ or Z_ C_ : Hole position data
Z_ or X_ : 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 the hole
Q_ : Depth of cut for each cutting feed F_ : The cutting feedrate
K_ : Number of repeats (when it is needed.)
d = Cutting start distance
M_ : M code for C-axis clamp (when it is needed.)
- Peck rigid tapping cycle
In the first cutting from point R, perform cutting by depth "q" specified by address Q while rotating the spindle in the forward direction (operation <1>).
Then, return to point R by rotating the spindle in the reverse direction (operation
<2>).
Then, rotate the spindle in the forward direction and perform cutting to the position indicated by [(Position to which cutting was performed previously) - (Cutting start distance set in parameter No. 5213)] as movement to the cutting start point (operation <3>).
Continue cutting by (d+q) (operation <4>).
Repeat operations <2> to <4> until the bottom of the hole is reached.
The cutting speed and rigid tapping time constant are used for operations <1> and
<4>.
For operations <2>, <3>, and travel from the bottom of the hole (point Z) to point R, rigid tapping extract override is enabled and the rigid tapping extract time constant is used.
Spindle stop
Point Z q
q Mα
(1) (2) d
Initial level
Spindle stop M(α+1) Point R P2
level Point R
(3)
(4)
d
d q
Spindle stop P1 Spindle CW
Spindle CCW Spindle stop
Spindle CCW Spindle stop Spindle CW
Point Z q
q Mα
(1)
d (2)
Spindle stop M(α+1) Point R P2
level Point R
(3)
(4)
d
d q
Spindle stop
Spindle stop P1 Spindle CW
Spindle CCW Spindle stop
Spindle CW
Spindle stop Spindle CCW
The symbols in the figure above indicate the following operations.
: Positioning (Rapid traverse G00) : Cutting feed (Linear interpolation G01) P1 : Dwell programmed by the address P command
Mα : Output of the M code for C-axis clamp (The α value is set in parameter No. 5110.) M(α+1) : Output of the M code for C-axis unclamp
P2 : Dwell set by parameter No.5111
Note P1, Mα, M(α+1), and P2 are not executed or output without being specified or set.
Explanation
- Cutting start distance
Cutting start distance d is set by parameter No. 5213.
- Amount of return
Amount of return for each time d is set by parameter No. 5213.
- Return speed
For the speed of return operation, a maximum of 2000% of override can be enabled by setting DOV (bit 4 of parameter No. 5200), OVU (bit 3 of parameter No. 5201), and parameter No. 5211 as with travel from the bottom of the hole (point Z) to point R.
- Speed during cutting into the cutting start point
For the speed during cutting into the cutting start point, a maximum of 2000% of override can be enabled by setting DOV (bit 4 of parameter No. 5200), OVU (bit 3 of parameter No. 5201), and parameter No.
5211 as with travel from the bottom of the hole (point Z) to point R.
- Acceleration/deceleration after interpolation
Linear or bell-shaped acceleration/deceleration can be applied.
- Look-ahead acceleration/deceleration before interpolation
Look-ahead acceleration/deceleration before interpolation is invalid.
- Override
Various types of override functions are invalid. The following override functions can be enabled by setting corresponding parameters:
• Extraction override
• Override signal Details are given later.
- Dry run
Dry run can be executed also in G84 (G88). When dry run is executed at the feedrate for the drilling axis in G84 (G88), tapping is performed according to the feedrate. Note that the spindle speed becomes faster at a higher dry run feedrate.
- Machine lock
Machine lock can be executed also in G84 (G88).
When G84 (G88) is executed in the machine lock state, the tool does not move along the drilling axis. Therefore, the spindle does not also rotate.
- Reset
When a reset is performed during rigid tapping, the rigid tapping mode is canceled and the spindle motor enters the normal mode. Note that the G84 (G88) mode is not canceled in this case when bit 6 (CLR) of parameter No. 3402 is set.
- Interlock
Interlock can also be applied in G84 (G88).
- Feed hold and single block
When parameter FHD (No. 5200#6) is set to 0, feed hold and single block are invalid in the G84 (G88) mode. When this bit is set to 1, they are valid.
- Manual feed
For rigid tapping by manual handle feed, see the section "Rigid Tapping by Manual Handle."
With other manual operations, rigid tapping cannot be performed.
- Backlash compensation
In the rigid tapping mode, backlash compensation is applied to compensate the lost motion when the spindle rotates clockwise or counterclockwise. Set the amount of backlash in parameters Nos. 5321 to 5324.
Along the drilling axis, backlash compensation has been applied.
- Series 10/11 format
When bit 1 (FCV) of parameter No. 0001 is set to 1, execution is enabled with G84.2. The same operation as with G84 is performed.
However, the command format for the repetitive count is L.
Limitation
- Axis switching
Before the drilling axis can be changed, the canned cycle must be canceled. If the drilling axis is changed in rigid mode, alarm PS0206 is issued.
- S commands
If a speed higher than the maximum speed for the gear being used is specified, alarm PS0200 is issued.
When the rigid tapping canned cycle is cancelled, the S command used for rigid tapping is cleared to S0.
- Distribution amount for the spindle
The maximum distribution amount is 32,767 pulses per 8 msec for a serial spindle. (displayed on diagnostic display No. 451)
This amount is changed according to the gear ratio setting for the position coder or rigid tapping command. If a setting is made to exceed the upper limit, alarm PS0202 is issued.
- F command
Specifying a value larger than the upper limit for cutting feed will cause alarm PS0011 to be issued.
- Unit of F command
Metric input Inch input Remarks G98 1mm/min 0.01inch/min Decimal point programming
allowed
G99 0.01mm/rev 0.0001inch/rev Decimal point programming allowed
- M29
If an S command and axis movement are specified between M29 and G84, alarm PS0203 is issued. If M29 is specified in a tapping cycle, alarm PS0204 is issued.
- Rigid tapping command M code
The M code used to specify the rigid tapping mode is set in parameter No. 5210.
- P/Q
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.
When Q0 is specified, the peck rigid tapping cycle is not performed.
- 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.
- Tool offset
In the canned cycle mode, tool offsets are ignored.
- Subprogram call
In the canned cycle mode, specify the subprogram call command M98P_ in an independent block.
- d (parameter No.5213)
Perform operation in the peck tapping cycle within point R. That is, set a value which does not exceed point R for d (parameter No. 5213).