Cycle 262 THREAD MILLING
ISO programming
G262
Application
With this cycle, you can mill a thread into pre-drilled material.
Related topics
- Cycle 263 THREAD MLLNG/CNTSNKG for milling a thread into pre-drilled material, optionally machining of a countersunk chamfer
- Cycle 264 THREAD DRILLNG/MLLNG for drilling into solid material and milling a thread, optionally machining of a countersunk chamfer
- Cycle 265 HEL. THREAD DRLG/MLG for milling a thread into solid material, optionally machining of a countersunk chamfer
- Cycle 267 OUTSIDE THREAD MLLNG for milling an external thread, optionally machining of a countersunk chamfer
Cycle run
- The control positions the tool in the spindle axis at rapid traverse FMAX to the entered set-up clearance above the workpiece surface
- 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.
- 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
- 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.
- After that the tool departs the contour tangentially and returns to the starting point in the working plane.
- At the end of the cycle, the control retracts the tool at rapid traverse to setup clearance or—if programmed—to 2nd setup clearance
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
- Enter depth as negative
- 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
- 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.
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.
11 CYCL DEF 262 THREAD MILLING ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 CYCL CALL |