Cycle 262 THREAD MILLING

ISO programming

G262

Application

With this cycle, you can mill a thread into pre-drilled material.

Related topics

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 moves at the programmed feed rate for pre-positioning to the starting plane. The starting plane is derived from the algebraic sign of the thread pitch, the milling method (climb or up-cut milling) and the number of threads per step.
  3. The tool then approaches the nominal thread diameter tangentially in a helical movement. Before the helical approach, a compensating movement of the tool axis is carried out in order to begin at the programmed starting plane for the thread path
  4. Depending on the setting of the parameter for the number of threads, the tool mills the thread in one helical movement, in several offset helical movements or in one continuous helical movement.
  5. After that the tool departs the contour tangentially and returns to the starting point in the working plane.
  6. At the end of the cycle, the control retracts the tool at rapid traverse to setup clearance or—if programmed—to 2nd setup clearance
 
Tip

The nominal thread diameter is approached in a semi-circle from the center. A pre-positioning movement to the side is carried out if the tool diameter is smaller than the nominal thread diameter by four times the thread pitch.

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
 
Notice
Danger of collision!
In the thread milling cycle, the tool will make a compensation movement in the tool axis before the approach. The length of the compensation movement is at most half of the thread pitch. This can result in a collision.
  1. Ensure sufficient space in the hole!
  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • If you change the thread depth, the control will automatically move the starting point for the helical movement.

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.
  • If you program the thread depth =0, the cycle will not be executed.

Cycle parameters

Help graphic

Parameter

Q335 Nominal diameter?

Nominal thread diameter

Input: 0...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

Q201 Depth of thread?

Distance between workpiece surface and root of thread. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q355 Number of threads per step?

Number of thread revolutions by which the tool is moved:

0 = one helical line to the thread depth

1 = continuous helical path over the entire length of the thread

>1 = several helical paths with approach and departure; between them, the control offsets the tool by Q355, multiplied by the pitch.

Input: 0...99999

Q253 Feed rate for pre-positioning?

Traversing speed of the tool in mm/min when plunging or when retracting.

Input: 0...99999.9999 or FMAX, FAUTO, PREDEF

Q351 Direction? Climb=+1, Up-cut=-1

Type of milling operation. The direction of spindle rotation is taken into account.

+1 = climb milling

–1 = up-cut milling

(if you enter 0, climb milling is performed)

Input: -1, 0, +1 or PREDEF

Q200 Set-up clearance?

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

Input: 0...99999.9999 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

Q207 Feed rate for milling?

Traversing speed of the tool in mm/min while milling

Input: 0...99999.999 or FAUTO

Q512 Feed rate for approaching? (optional)

Traversing speed of the tool in mm/min while approaching. For smaller thread diameters, you can decrease the approaching feed rate in order to reduce the danger of tool breakage.

Input: 0...99999.999 or FAUTO

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 262 THREAD MILLING ~

Q335=+5

;NOMINAL DIAMETER ~

Q239=+1

;THREAD PITCH ~

Q201=-18

;DEPTH OF THREAD ~

Q355=+0

;THREADS PER STEP ~

Q253=+750

;F PRE-POSITIONING ~

Q351=+1

;CLIMB OR UP-CUT ~

Q200=+2

;SET-UP CLEARANCE ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+50

;2ND SET-UP CLEARANCE ~

Q207=+500

;FEED RATE MILLING ~

Q512=+0

;FEED FOR APPROACH

12 CYCL CALL