ISO programming
G253
G253
Use Cycle 253 to completely machine a slot. Depending on the cycle parameters, the following machining alternatives are available:
Roughing
Finishing
Help graphic | Parameter |
---|---|
Q215 Machining operation (0/1/2)? Define the machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing Input: 0, 1, 2 | |
Q218 Length of slot? Enter the length of the slot. It is parallel to the main axis of the working plane. Input: 0...99999.9999 | |
Q219 Width of slot? Enter the width of the slot, which must be parallel to the secondary axis of the working plane. If the slot width equals the tool diameter, the control will mill an oblong hole. Maximum slot width for roughing: Twice the tool diameter Input: 0...99999.9999 | |
Q368 Finishing allowance for side? Finishing allowance in the working plane. This value has an incremental effect. Input: 0...99999.9999 | |
Q374 Angle of rotation? Angle by which the entire slot is rotated. The center of rotation is the position at which the tool is located when the cycle is called. This value has an absolute effect. Input: –360.000...+360.000 | |
Q367 Position of slot (0/1/2/3/4)? Position of the figure relative to the position of the tool when the cycle is called: 0: Tool position = Center of figure 1: Tool position = Left end of figure 2: Tool position = Center of left figure arc 3: Tool position = Center of right figure arc 4: Tool position = Right end of figure Input: 0, 1, 2, 3, 4 | |
Q207 Feed rate for milling? Traversing speed of the tool in mm/min for milling Input: 0...99999.999 or FAUTO, FU, FZ | |
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 PREDEF: The control uses the value of a GLOBAL DEF block (If you enter 0, climb milling is performed) Input: -1, 0, +1 or PREDEF | |
Q201 Depth? Distance between workpiece surface and slot floor. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
Q202 Plunging depth? Tool infeed per cut. Enter a value greater than 0. This value has an incremental effect. Input: 0...99999.9999 | |
Q369 Finishing allowance for floor? Finishing allowance for the floor. This value has an incremental effect. Input: 0...99999.9999 | |
Q206 Feed rate for plunging? Traversing speed of the tool in mm/min for moving to depth Input: 0...99999.999 or FAUTO, FU, FZ | |
Q338 Infeed for finishing? Tool infeed in the spindle axis per finishing cut. Q338 = 0: Finishing with a single infeed 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? Coordinate in the spindle axis at which a collision between tool and workpiece (fixtures) is impossible. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
Q366 Plunging strategy (0/1/2)? Type of plunging strategy: 0 = Vertical plunging. The plunging angle ANGLE in the tool table is not evaluated. 1, 2= Reciprocating plunge. In the tool table, the plunging angle ANGLE for the active tool must be defined as not equal to 0. Otherwise, the control will display an error message. Alternative: PREDEF Input: 0, 1, 2 | |
Q385 Finishing feed rate? Traversing speed of the tool in mm/min for side and floor finishing Input: 0...99999.999 or FAUTO, FU, FZ | |
Q439 Feed rate reference (0-3)? Specify the reference for the programmed feed rate: 0: Feed rate is referenced to the path of the tool center 1: Feed rate is referenced to the cutting edge only during side finishing; otherwise, it is referenced to the path of the tool center 2: Feed rate is referenced to the cutting edge during side finishing and floor finishing; otherwise it is referenced to the path of the tool center 3: Feed rate is always referenced to the cutting edge Input: 0, 1, 2, 3 |
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 253 SLOT MILLING ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 L X+50 Y+50 R0 FMAX M99 |