ISO programming
G262
G262
With this cycle, you can mill a thread into pre-drilled material.
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.
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? 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.
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 |