Cycle 18 THREAD CUTTING

ISO programming

G86

Application

Cycle 18 THREAD CUTTING moves the tool with servo-controlled spindle from the momentary position with active speed to the specified depth. As soon as it reaches the end of thread, spindle rotation is stopped. Approach and departure movements must be programmed separately.

Notes

 
Machine

Cycle 18 THREAD CUTTING can be hidden with the optional machine parameter hideRigidTapping (no. 128903).

 
Notice
Danger of collision!
If you do not program a pre-positioning step before programming the call of Cycle 18, a collision might occur. Cycle 18 does not perform any approach or departure movements.
  1. Pre-position the tool before the start of the cycle.
  2. The tool moves from the current position to the entered depth after the cycle is called
 
Notice
Danger of collision!
If the spindle was switched on before the start of this cycle, Cycle 18 will switch it off and the cycle will execute with a stationary spindle! At the end, Cycle 18 will switch the spindle on again if it was on before the start of the cycle.
  1. Before starting this cycle, be sure to program a spindle stop! (For example with M5)
  2. 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.

 
Tip

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.

Example

11 CYCL DEF 18.0 THREAD CUTTING

12 CYCL DEF 18.1 DEPTH-20

13 CYCL DEF 18.2 PITCH+1