- Q command
After setting bit 6 (PCT) of parameter No. 5104 to 1, add address Q to the ordinary tapping cycle command format and specify the depth of cut for each tapping.
In the peck tapping cycle, the tool is retracted to point R for each tapping. In the high-speed peck tapping cycle, the tool is retracted by the retraction distance specified for parameter No. 5213 in advance.
Which operation is to be performed can be selected by setting bit 5 (PCP) of parameter No. 5200.
Operation
First, ordinary tapping cycle operation is explained as basic operation.
Before specifying a tapping cycle, rotate the spindle using a miscellaneous function.
1. When a command to position the tool to a hole position, positioning is performed.
2. When point R is specified, positioning to point R is performed.
3. Tapping is performed to the bottom of the hole in cutting feed.
4. When a dwell time (P) is specified, the tool dwells.
5. Miscellaneous function M05 (spindle stop) is output and the machine enters the FIN wait state.
6. When FIN is returned, miscellaneous function M04 (reverse spindle rotation) is output and the machine enters the FIN wait state.
7. When FIN is returned, the tap is removed until point R is reached in cutting feed.
8. When a dwell time (P) is specified, the tool dwells.
9. Miscellaneous function M05 (spindle stop) is output and the machine enters the FIN wait state.
10. When FIN is returned, miscellaneous function M03 (forward spindle rotation) is output, and the machine enters the FIN wait state.
11. When FIN is returned, the tool returns to the initial point in rapid traverse when return to the initial level is specified.
When the repetitive count is specified, operation is repeated from step 1.
<1> Positioning to a hole
<2> Positioning to point R
Point R level
Hole bottom level
<3> Tapping to the bottom of the hole
<4> Dwell
<5> Output of miscellaneous function M05
<6> Output of miscellaneous function M04
<7> Return to point R
<8> Dwell
<9> Output of miscellaneous function M05
<10> Output of miscellaneous function M03
<11> Positioning to the initial point
<1> Positioning to the next hole
Workpiece
Tapping
Peck tapping cycle
When bit 6 (PCT) of parameter No. 5104 is set 1 and bit 5 (PCP) of parameter No. 5200 is set to 1, the peck tapping cycle is used.
Step 3 of the tapping cycle operation described above changes as follows:
3-1. The tool cuts the workpiece by the depth of cut q specified by address Q.
3-2. Miscellaneous function M05 (spindle stop) is output, and the machine enters the FIN wait state.
3-3. When FIN is returned, miscellaneous function M04 (reverse spindle rotation) is output, and the machine enters the FIN wait state.
3-4. When FIN is returned, the tool is retracted to point R in cutting feed.
3-5. Miscellaneous function M05 (spindle stop) is output, and the machine enters the FIN wait state.
3-6. When FIN is returned, miscellaneous function M03 (forward spindle rotation) is output, and the machine enters the FIN wait state.
3-7. When FIN is returned, the tool moves to the position the clearance d (parameter No. 5213) apart from the previous cutting point in cutting feed (approach).
3-1. The tool cuts the workpiece by the clearance d (parameter No.
5213) + depth of cut q (specified by address Q).
Tapping is performed to the bottom of the hole by repeating the above steps.
When a dwell time (P) is specified, the tool dwells only when it reaches at the bottom of the hole and reaches point R last.
Point R level
Hole bottom level Workpiece
q
d
q
q
<2> Output of miscellaneous function M05
<3> Output of miscellaneous function M04
<5> Output of miscellaneous function M05
<6> Output of miscellaneous function M03
<1> Tapping
<1> Tapping
<1> Tapping
<4> Retraction
<4> Retraction
d
<7> Approach
Repeated until the bottom of the hole is reached.
q: Depth of cut d: Clearance
<7> Approach
High-speed peck tapping cycle
When bit 6 (PCT) of parameter No. 5104 is set 1 and bit 5 (PCP) of parameter No. 5200 is set to 0, the high-speed peck tapping cycle is used.
Step 3 of the tapping cycle operation described above changes as follows:
3-1. The tool cuts the workpiece by the depth of cut q specified by address Q.
3-2. Miscellaneous function M05 (spindle stop) is output, and the machine enters the FIN wait state.
3-3. When FIN is returned, miscellaneous function M04 (reverse spindle rotation) is output, and the machine enters the FIN wait state.
3-4. When FIN is returned, the tool is retracted by the retraction distance d specified by parameter No. 5213 in cutting feed.
3-5. Miscellaneous function M05 (spindle stop) is output, and the machine enters the FIN wait state.
3-6. When FIN is returned, miscellaneous function M03 (forward spindle rotation) is output, and the machine enters the FIN wait state.
3-1. When FIN is returned, the tool cuts the workpiece by the retraction distance d (parameter No. 5213) + depth of cut q (specified by address Q).
Tapping is performed to the bottom of the hole by repeating the above steps.
When a dwell time (P) is specified, the tool dwells only when it reaches at the bottom of the hole and reaches point R.
Point R level
Hole bottom level Workpiece
q d
q
d
q
<2> Output of miscellaneous function M05
<3> Output of miscellaneous function M04
<5> Output of miscellaneous function M05
<6> Output of miscellaneous function M03
<1> Tapping
<1> Tapping
<1> Tapping
<4> Retraction
<4> Retraction
Repeated until the bottom of the hole is reached.
q: Depth of cut d: Retraction distance
Notes
1. The depth of cut specified by address Q is stored as a modal value until the canned cycle mode is canceled.
In both examples 1 and 2 below, address Q is not specified in the N20 block, but the peck tapping cycle is performed because the value specified by address Q is valid as a modal value. If this operation is not suitable, specify G80 to cancel the canned cycle mode as shown in N15 in example 3 or specify Q0 in the tapping block as shown in N20 in example 4.
Example 1
N10 G84 X100. Y150. Z-100. Q20. ;
N20 X150. Y200 ; q The peck tapping cycle is also performed in this block.
N30 G80 ;
Example 2
N10 G83 X100. Y150. Z-100. Q20. ;
N20 G84 Z-100. ; q The peck tapping cycle is also performed in this block.
N30 G80 ;
Example 3
N10 G83 X100. Y150. Z-100. Q20. ;
N15 G80 ; q The canned cycle mode is canceled.
N20 G84 Z-100. ; N30 G80 ;
Example 4
N10 G83 X100. Y150. Z-100. Q20. ; N20 G84 Z-100. Q0 ; qQ0 is added.
N30 G80 ;
2. The unit for the reference axis that is set by parameter No. 1031, not the unit for the drilling axis is used as the unit of Q. Any sign is ignored.
3. Specify a radius value at address Q even when a diameter axis is used.
4. 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).
Example
M51 ; Setting C-axis index mode ON
M3 S2000 ; Rotating the drill
G00 X50.0 C0.0 ; Positioning the drill along the X- and C- axes
G84 Z-40.0 R-5.0 P500 F5.0 M31 ; Drilling hole 1
C90.0 M31 ; Drilling hole 2
C180.0 M31 ; Drilling hole 3
C270.0 M31 ; Drilling hole 4
G80 M05 ; Canceling the drilling cycle and
stopping drill rotation
M50 ; Setting C-axis index mode off
4.3.3 Front Boring Cycle (G85) / Side Boring Cycle (G89)
This cycle is used to bore a hole.
Format
G85 X(U)_ C(H)_ Z(W)_ R_ P_ F_ K_ M_ ; or
G89 Z(W)_ C(H)_ X(U)_ R_ P_ 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 a hole
F_ : Cutting feedrate
K_ : Number of repeats (When it is needed.) M_ : M code for C-axis clamp (When it is needed.)
G85 or G89 (G98 mode) G85 or G89 (G99 mode)
Point R
Point Z Initial level
M (α + 1), P2 Mα
P1
Point R
Point Z Point R level Mα
P1
M (α + 1), P2
Mα : M code for C-axis clamp M (α + 1) : M code for C-axis unclamp P1 : Dwell specified in the program
P2 : Dwell specified in parameter No. 5111 Explanation
After positioning, rapid traverse is performed to point R.
Drilling is performed from point R to point Z.
After the tool reaches point Z, it returns to point R at a feedrate twice the cutting feedrate.
Example
M51 ; Setting C-axis index mode ON
M3 S2000 ; Rotating the drill
G00 X50.0 C0.0 ; Positioning the drill along the X- and C-axes
G85 Z-40.0 R-5.0 P500 F5.0 M31 ; Drilling hole 1
C90.0 M31 ; Drilling hole 2
C180.0 M31 ; Drilling hole 3
C270.0 M31 ; Drilling hole 4
G80 M05 ; Canceling the drilling cycle and
stopping drill rotation
M50 ; Setting C-axis index mode off
4.3.4 Canned Cycle for Drilling Cancel (G80)
G80 cancels canned cycle for drilling.
Format
G80 ;
Explanation
Canned cycle for drilling is canceled to perform normal operation.
Point R and point Z are cleared.
Other drilling data is also canceled (cleared).
Example
M51 ; Setting C-axis index mode ON
M3 S2000 ; Rotating the drill
G00 X50.0 C0.0 ; Positioning the drill along the X- and C-axes.
G83 Z-40.0 R-5.0 P500 F5.0 M31 ; Drilling hole 1
C90.0 M31 ; Drilling hole 2
C180.0 M31 ; Drilling hole 3
C270.0 M31 ; Drilling hole 4
G80 M05 ; Canceling the drilling cycle and
stopping drill rotation
M50 ; Setting C-axis index mode off
4.3.5 Precautions to be Taken by Operator
- Reset and emergency stop
Even when the controller is stopped by resetting or emergency stop in the course of drilling cycle, the drilling mode and drilling data are saved; with this mind, therefore, restart operation.
- Single block
When drilling cycle is performed with a single block, the operation stops at the end points of operations 1, 2, 6 in Fig. 4.3 (a).
Consequently, it follows that operation is started up 3 times to drill one hole. The operation stops at the end points of operations 1, 2 with the feed hold lamp ON. If there is a remaining repetitive count at the end of operation 6, the operation is stopped by feed hold. If there is no remaining repetitive count, the operation is stopped in the single block stop state.
- Feed hold
When "Feed Hold" is applied between operations 3 and 5 by G84/G88, the feed hold lamp lights up immediately if the feed hold is applied again to operation 6.
- Override
During operation with G84 and G88, the feedrate override is 100%.
4.4 RIGID TAPPING
Front face tapping cycles (G84) and side face tapping cycles (G88) can be performed either in conventional mode or rigid mode.
In conventional mode, the spindle is rotated or stopped, in synchronization with the motion along the tapping axis according to miscellaneous functions M03 (spindle CW rotation), M04 (spindle CCW rotation), and M05 (spindle stop).
In rigid mode, the spindle motor is controlled in the same way as a control motor, by the application of compensation to both motion along the tapping axis and that of the spindle.
For rigid tapping, each turn of the spindle corresponds to a certain amount of feed (screw lead) along the spindle axis. This also applies to acceleration/deceleration. This means that rigid tapping does not demand the use of float tappers as in the case of conventional tapping, thus enabling high-speed, high-precision tapping.
When multispindle control is enabled (bit 3 (MSP) of parameter No.
8133 is set to 1), the second spindle can be used for rigid tapping.