ISO programming
G264
G264
With this cycle, you can drill into solid material, machine a counterbore, and finally mill a thread.
Drilling
Countersinking at front
Thread milling
Program the thread depth as a value smaller than the total hole depth by at least one-third 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 | |
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.
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? 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 264 THREAD DRILLNG/MLLNG ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 CYCL CALL |