Cycle 207 RIGID TAPPING

ISO programming

G207

Application

 
Machine

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 control cuts the thread without a floating tap holder in one or more passes.

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. The direction of spindle rotation is then reversed and the tool is retracted to set-up clearance. If programmed, the tool moves to the 2nd set-up clearance at FMAX.
  4. The control stops the spindle rotation at set-up clearance.
 
Tip

For tapping, the spindle and the tool axis are always synchronized with each other. The synchronization can be carried out while the spindle is rotating or while it is stationary.

Notes

 
Machine

Cycle 207 RIGID TAPPING can be hidden with the optional machine parameter hideRigidTapping (no. 128903).

 
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.
  • 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.
 
Tip

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 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): 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

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

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 207 RIGID TAPPING ~

Q200=+2

;SET-UP CLEARANCE ~

Q201=-18

;DEPTH OF THREAD ~

Q239=+1

;THREAD PITCH ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+50

;2ND SET-UP CLEARANCE

12 CYCL CALL

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.