Cycle 18 THREAD CUTTING
ISO programming
G86
Application
Related topics
- Cycles for Thread Machining
Notes
Cycle 18 THREAD CUTTING can be hidden with the optional machine parameter hideRigidTapping (no. 128903).
- Pre-position the tool before the start of the cycle.
- The tool moves from the current position to the entered depth after the cycle is called
- Before starting this cycle, be sure to program a spindle stop! (For example with M5)
- At the end of Cycle 18, the control restores the spindle to its state at cycle start. This means that if the spindle was switched off before this cycle, the control will switch it off again at the end of Cycle 18.
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
Notes on programming
- Before calling this cycle, program a spindle stop (for example with M5). The control automatically activates spindle rotation at the start of the cycle and deactivates it at the end.
- The algebraic sign for the cycle parameter "thread depth" determines the working direction.
Note regarding machine parameters
- Use machine parameter CfgThreadSpindle (no. 113600) to define the following:
- sourceOverride (no. 113603): Spindle potentiometer (feed rate override is not active) and feed potentiometer (spindle speed override is not active); the control then adjusts the spindle speed as required
- 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.
- limitSpindleSpeed (no. 113604): Spindle speed limit
True: At small thread depths, spindle speed is limited so that the spindle runs with a constant speed approx. 1/3 of the time.
False: Limiting not active
Cycle parameters
Help graphic | Parameter |
---|---|
Total hole depth? Enter the thread depth relative to the current position. This value has an incremental effect. Input: –999999999...+999999999 | |
Thread pitch? Enter the thread pitch. The algebraic sign entered here differentiates between right-hand and left-hand threads: + = Right-hand thread (M3 with negative hole depth) – = Left-hand thread (M4 with negative hole depth) Input: –99.9999...+99.9999 |
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 18.0 THREAD CUTTING |
12 CYCL DEF 18.1 DEPTH-20 |
13 CYCL DEF 18.2 PITCH+1 |