Cycle 264 THREAD DRILLNG/MLLNG

ISO programming

G264

Application

With this cycle, you can drill into solid material, machine a counterbore, and finally mill a 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

Drilling

  1. The tool drills to the first plunging depth at the programmed feed rate for plunging.
  2. If you have programmed chip breaking, the tool then retracts by the entered retraction value. If you are working without chip breaking, the tool is retracted at rapid traverse to set-up clearance, and then moved again at FMAX to the entered advanced stop distance above the first plunging depth
  3. The tool then advances with another infeed at the programmed feed rate.
  4. The control repeats this procedure (steps 2 to 4) until the total drilling depth is reached

Countersinking at front

  1. The tool moves at the feed rate for pre-positioning to the sinking depth at front.
  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. The starting plane is determined from the algebraic sign of the thread pitch and the type of milling (climb or up-cut)
  2. Then the tool moves tangentially on a helical path to the thread diameter and mills the thread with a 360° helical motion
  3. After that the tool departs the contour tangentially and returns to the starting point in the working plane.
  4. 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.
  • The algebraic sign of the cycle parameters thread depth, countersinking depth or depth at front determines the working direction. The working direction is defined in the following sequence:
    1. Depth of thread
    2. Countersinking depth
    3. 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.
 
Tip

Program the thread depth as a value smaller than the total hole depth by at least one-third the thread pitch.

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

Q356 Total hole depth?

Distance between workpiece surface and hole bottom. 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

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

Q202 Maximum plunging depth?

Infeed per cut. The DEPTH Q201 does not have to be a multiple of Q202. This value has an incremental effect.

The depth does not have to be a multiple of the plunging depth. The control will go to depth in one movement if:

  • the plunging depth is equal to the depth
  • the plunging depth is greater than the depth

Input: 0...99999.9999

Q258 Upper advanced stop distance?

Safety clearance above the last plunging depth to which the tool returns at Q373 FEED AFTER REMOVAL after first chip removal. This value has an incremental effect.

Input: 0...99999.9999

Q257 Infeed depth for chip breaking?

Incremental depth at which the control performs chip breaking. This procedure is repeated until DEPTH Q201 is reached. If Q257 equals 0, the control will not perform chip breaking. This value has an incremental effect.

Input: 0...99999.9999

Q256 Retract dist. for chip breaking?

Value by which the control retracts the tool during chip breaking. This value has an incremental effect.

Input: 0...99999.999 or 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

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

Q206 Feed rate for plunging?

Tool traversing speed in mm/min during plunging

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

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 264 THREAD DRILLNG/MLLNG ~

Q335=+5

;NOMINAL DIAMETER ~

Q239=+1

;THREAD PITCH ~

Q201=-18

;DEPTH OF THREAD ~

Q356=-20

;TOTAL HOLE DEPTH ~

Q253=+750

;F PRE-POSITIONING ~

Q351=+1

;CLIMB OR UP-CUT ~

Q202=+5

;PLUNGING DEPTH ~

Q258=+0.2

;UPPER ADV STOP DIST ~

Q257=+0

;DEPTH FOR CHIP BRKNG ~

Q256=+0.2

;DIST FOR CHIP BRKNG ~

Q358=+0

;DEPTH AT FRONT ~

Q359=+0

;OFFSET AT FRONT ~

Q200=+2

;SET-UP CLEARANCE ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+50

;2ND SET-UP CLEARANCE ~

Q206=+150

;FEED RATE FOR PLNGNG ~

Q207=+500

;FEED RATE MILLING ~

Q512=+0

;FEED FOR APPROACH

12 CYCL CALL