Cycle 206 TAPPING

ISO programming

G206

Application

The thread is cut in one or more passes. A floating tap holder is used.

Cycle run

  1. The control positions the tool in the spindle axis at rapid traverse FMAX to the entered set-up clearance above the workpiece surface.
  2. The tool taps to the total hole depth in one movement.
  3. Once the tool has reached this position, the direction of spindle rotation is reversed and the tool is retracted to set-up clearance at the end of the dwell time. If programmed, the tool moves to the 2nd set-up clearance at FMAX.
  4. At the set-up clearance, the direction of spindle rotation is reversed once again.
 
Tip

A floating tap holder is required for tapping. It must compensate for the tolerances between feed rate and spindle speed during the tapping process.

Notes

 
Notice
Danger of collision!
If you enter the depth in a cycle as a positive value, the control reverses the calculation of the pre-positioning. The tool moves at rapid traverse in the tool axis to set-up the clearance below the workpiece surface! There is a danger of collision!
  1. Enter depth as negative
  2. 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.
  • For tapping right-hand threads activate the spindle with M3, for left-hand threads use M4.
  • In Cycle 206, the control uses the programmed rotational speed and the feed rate defined in the cycle to calculate the thread pitch.
  • 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.

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 DEPTH cycle parameter determines the working direction. If you program DEPTH=0, the cycle will not be executed.

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.

Cycle parameters

Help graphic

Parameter

Q200 Set-up clearance?

Distance between tool tip and workpiece surface. This value has an incremental effect.

Guide value: 4 times the thread pitch

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

Q206 Feed rate for plunging?

Traversing speed of the tool during tapping

Input: 0...99999.999 or FAUTO

Q211 Dwell time at the depth?

Enter a value between 0 and 0.5 seconds to avoid wedging of the tool during retraction.

Input: 0...3600.0000 or PREDEF

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

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 206 TAPPING ~

Q200=+2

;SET-UP CLEARANCE ~

Q201=-18

;DEPTH OF THREAD ~

Q206=+150

;FEED RATE FOR PLNGNG ~

Q211=+0

;DWELL TIME AT DEPTH ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+50

;2ND SET-UP CLEARANCE

12 CYCL CALL

The feed rate is calculated as follows: F = S x p

F:

Feed rate (mm/min)

S:

Spindle speed (rpm)

p:

Thread pitch (mm)

Retraction with stopped NC program

You can retract a thread-turning tool as follows in stopped state:

  1. Select Tool Retract

  1. Press the NC Start key
  2. The tool retracts from the hole and moves to the starting point of machining.
  3. The spindle is stopped automatically. The control issues an error message.
  4. Cancel the NC program with the INTERNAL STOP button
  5. or

  6. Acknowledge the error message and continue with NC Start
 
Tip
  • 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.