Cycle 265 HEL. THREAD DRLG/MLG

ISO programming

G265

Application

With this cycle, you can mill a thread into solid material. In addition, you can choose to machine a counterbore before or after milling the thread.

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

Countersinking at front

  1. If countersinking occurs before thread milling, the tool moves at the feed rate for countersinking to the sinking depth at front. If countersinking occurs after thread milling, the control moves the tool to the countersinking depth at the feed rate for prepositioning
  2. The control positions the tool without compensation from its center position on a semicircle to the offset at front, and then follows a circular path at the feed rate for countersinking
  3. The tool then moves in a semicircle to the hole center

Thread milling

  1. The control moves the tool at the programmed feed rate for pre-positioning to the starting plane for the thread
  2. The tool then approaches the nominal thread diameter tangentially in a helical movement
  3. The tool moves on a continuous helical downward path until the thread depth value is reached
  4. After that the tool departs the contour tangentially and returns to the starting point in the working plane.
  5. At the end of the cycle, the control retracts the tool at rapid traverse to setup clearance or—if programmed—to 2nd setup clearance

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.
  • If you change the thread depth, the control will automatically move the starting point for the helical movement.
  • The type of milling (up-cut or climb) is determined by the thread (right-hand or left-hand thread) and the direction of tool rotation, since it is only possible to work in the direction of the tool.
  • The algebraic sign of the cycle parameters depth of thread or sinking depth at front determines the working direction. The working direction is defined in the following sequence:
    1. Depth of thread
    2. Depth at front

Notes on programming

  • Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0.
  • If you program one of the depth parameters to be 0, the control does not execute that step.

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

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

Q358 Sinking depth at front?

Distance between tool point and the top surface of the workpiece for countersinking at the front of the tool. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q359 Countersinking offset at front?

Distance by which the control moves the tool center away from the center. This value has an incremental effect.

Input: 0...99999.9999

Q360 Countersink (before/after:0/1)?

Execution of the chamfer

0 = before thread machining

1 = after thread machining

Input: 0, 1

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

Q254 Feed rate for counterboring?

Traversing speed of the tool in mm/min during counterboring

Input: 0...99999.999 or FAUTO, FU

Q207 Feed rate for milling?

Traversing speed of the tool in mm/min while milling

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 265 HEL. THREAD DRLG/MLG ~

Q335=+5

;NOMINAL DIAMETER ~

Q239=+1

;THREAD PITCH ~

Q201=-18

;DEPTH OF THREAD ~

Q253=+750

;F PRE-POSITIONING ~

Q358=+0

;DEPTH AT FRONT ~

Q359=+0

;OFFSET AT FRONT ~

Q360=+0

;COUNTERSINK PROCESS ~

Q200=+2

;SET-UP CLEARANCE ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+50

;2ND SET-UP CLEARANCE ~

Q254=+200

;F COUNTERBORING ~

Q207=+500

;FEED RATE MILLING

12 CYCL CALL