Cycle 209 TAPPING W/ CHIP BRKG
ISO programming
G209
Application
Refer to your machine manual.
Machine and control must be specially prepared by the machine manufacturer for use of this cycle.
This cycle is effective only for machines with servo-controlled spindle.
The tool machines the thread in several passes until it reaches the programmed depth. You can define in a parameter whether the tool is to be retracted completely from the hole for chip breaking.
Related topics
- Cycle 206 TAPPING with floating tap holder
- Cycle 207 RIGID TAPPING without floating tap holder
Cycle run
- The control positions the tool in the tool axis at rapid traverse FMAX to the programmed set-up clearance above the workpiece surface.There, it carries out an oriented spindle stop
- The tool moves to the programmed infeed depth, reverses the direction of spindle rotation and retracts by a specific distance or completely for chip release, depending on the definition. If you have defined a factor for increasing the spindle speed, the control retracts from the hole at the corresponding speed
- It then reverses the direction of spindle rotation again and advances to the next infeed depth.
- The control repeats this procedure (steps 2 to 3) until the programmed thread depth is reached
- The tool is then retracted to set-up clearance. If programmed, the tool moves to 2nd set-up clearance at FMAX
- The control stops the spindle turning at that set-up clearance
For tapping, the spindle and the tool axis are always synchronized with each other. Synchronization may take place while the spindle is stationary.
Notes
Cycle 209 TAPPING W/ CHIP BRKG can be hidden with the optional machine parameter hideRigidTapping (no. 128903).
- Enter depth as negative
- Use the machine parameter displayDepthErr (no. 201003) to specify whether the control should display an error message (on) or not (off) if a positive depth is entered
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- If you program M3 (or M4) before this cycle, the spindle rotates after the end of the cycle (at the speed programmed in the TOOL CALL block).
- If you do not program M3 (or M4) before this cycle, the spindle will stand still after the end of the cycle. In this case, you must restart the spindle with M3 (or M4) before the next operation.
- If you enter the thread pitch of the tap in the Pitch column of the tool table, the control compares the thread pitch from the tool table with the thread pitch defined in the cycle. If the values do not match, the control displays an error message.
- This cycle monitors the defined usable length LU of the tool. If it is less than the DEPTH OF THREAD Q201, the control will display an error message.
If you do not change any dynamic parameters (e.g., set-up clearance, spindle speed,...), it is possible to later tap the thread to a greater depth. However, make sure to select a set-up clearance Q200 that is large enough so that the tool axis leaves the acceleration path within this distance.
Notes on programming
- Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0.
- The algebraic sign for the cycle parameter "thread depth" determines the working direction.
- If you defined a speed factor for fast retraction in cycle parameter Q403, the control limits the speed to the maximum speed of the active gear stage.
Note regarding machine parameters
- Use machine parameter CfgThreadSpindle (no. 113600) to define the following:
- sourceOverride (no. 113603):
FeedPotentiometer (default) (speed override is not active), the control then adjusts the speed as required
SpindlePotentiometer (feed rate override is not active) - thrdWaitingTime (no. 113601): After the spindle stop, the tool will dwell at the bottom of the thread for the time specified
- thrdPreSwitch (no. 113602): The spindle is stopped for this period of time before reaching the bottom of the thread.
- sourceOverride (no. 113603):
Cycle parameters
Help graphic | Parameter |
---|---|
Q200 Set-up clearance? Distance between tool tip and workpiece surface. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
Q201 Depth of thread? Distance between workpiece surface and root of thread. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
Q239 Pitch? Pitch of the thread. The algebraic sign differentiates between right-hand and left-hand threads: += right-hand thread – = left-hand thread Input: –99.9999...+99.9999 | |
Q203 Workpiece surface coordinate? Coordinate on the workpiece surface referenced to the active datum. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q204 2nd set-up clearance? Distance in the tool axis between tool and workpiece (fixtures) at which no collision can occur. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
Q257 Infeed depth for chip breaking? Incremental depth at which the control performs chip breaking. This procedure is repeated until DEPTH Q201 is reached. If Q257 equals 0, the control will not perform chip breaking. This value has an incremental effect. Input: 0...99999.9999 | |
Q256 Retract dist. for chip breaking? The control multiplies the pitch Q239 by the programmed value and retracts the tool by the calculated value during chip breaking. If you enter Q256 = 0, the control retracts the tool completely from the hole (to set-up clearance) for chip breaking. Input: 0...99999.9999 | |
Q336 Angle for spindle orientation? Angle to which the control positions the tool before machining the thread. This value has an absolute effect. Input: 0...360 | |
Q403 RPM factor for retraction? (optional) Factor by which the control increases the spindle speed—and therefore also the retraction feed rate—when retracting from the drill hole. Maximum increase to maximum speed of the active gear stage. Input: 0.0001...10 |
NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.
Change the following contents as needed:
- Tools
- Cutting parameters
- Feed rates
- Clearance height or safe position
- Machine-specific positions (e.g., with M91)
- Paths of program calls
Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.
In addition, test the NC programs using the simulation before the actual program run.
With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.
11 CYCL DEF 209 TAPPING W/ CHIP BRKG ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 CYCL CALL |
Retraction with stopped NC program
You can retract a thread-turning tool as follows in stopped state:
| ||
|
- Program Run operating mode:
When stopping the NC program with NC stop, the control displays the Tool Retract button.
- MDI application:
When you call a thread cycle, the Tool Retract button appears. The button is grayed out until you press NC stop.