ISO programming
G251
G251
Use Cycle 251 to completely machine rectangular pockets. 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 First side length? Pocket length, parallel to the main axis of the working plane. This value has an incremental effect. Input: 0...99999.9999 | |
Q219 Second side length? Pocket length, parallel to the secondary axis of the working plane. This value has an incremental effect. Input: 0...99999.9999 | |
Q220 Corner radius? Radius of the pocket corner. If you have entered 0 here, the control assumes that the corner radius is equal to the tool radius. 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 | |
Q224 Angle of rotation? Angle by which the entire operation 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 pocket (0/1/2/3/4)? Position of the pocket with respect to the tool when the cycle is called: 0: Tool position = Center of pocket 1: Tool position = Lower left corner 2: Tool position = Lower right corner 3: Tool position = Upper right corner 4: Tool position = Upper left corner 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 bottom of pocket. 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 | |
Q370 Path overlap factor? Q370 x tool radius = stepover factor k. Input: 0.0001...1.41 or PREDEF | |
Q366 Plunging strategy (0/1/2)? Type of plunging strategy: 0: Vertical plunging. The control plunges perpendicularly, regardless of the plunging angle ANGLE defined in the tool table. 1: Helical plunging. 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. If necessary, define the value of the RCUTS cutting width in the tool table 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. The reciprocation length depends on the plunging angle. As a minimum value, the control uses twice the tool diameter. If necessary, define the value of the RCUTS cutting width in the tool table PREDEF: The control uses the value from the GLOBAL DEF block Input: 0, 1, 2 or PREDEF | |
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 251 RECTANGULAR POCKET ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 L X+50 Y+50 R0 FMAX M99 |
Rcorr: Tool radius R + tool radius oversize DR