ISO programming
G258
G258
Use Cycle 258 to machine a regular polygon by machining the contour outside. The milling operation is carried out on a spiral path based on the diameter of the workpiece blank.
Help graphic | Parameter |
---|---|
Q573 Inscr.circle/circumcircle (0/1)? Define whether the dimension Q571 is referenced to the inscribed circle or the circumcircle: 0: Dimension is referenced to the inscribed circle 1: Dimension is referenced to the circumcircle Input: 0, 1 | |
Q571 Reference circle diameter? Enter the diameter of the reference circle. Specify in parameter Q573 whether the diameter entered here is referenced to the inscribed circle or the circumcircle. You can program a tolerance if needed. Input: 0...99999.9999 | |
Q222 Workpiece blank diameter? Enter the diameter of the blank. The workpiece blank diameter must be greater than the reference circle diameter. The control performs multiple stepovers if the difference between the workpiece blank diameter and reference circle diameter is greater than the permitted stepover (tool radius multiplied by path overlap Q370). The control always calculates a constant stepover. Input: 0...99999.9999 | |
Q572 Number of corners? Enter the number of corners of the polygon stud. The control distributes the corners evenly on the stud. Input: 3...30 | |
Q224 Angle of rotation? Specify which angle is used to machine the first corner of the polygon stud. Input: –360.000...+360.000 | |
Q220 Radius / Chamfer (+/-)? Enter the value for the radius or chamfer form element. If you enter a positive value, the control will round every corner. The value you enter here refers to the radius. If you enter a negative value, all corners of the contour will be chamfered with the value entered as the length of the chamfer. Input: –99999.9999...+99999.9999 | |
Q368 Finishing allowance for side? Finishing allowance in the working plane. If you enter a negative value here, the control will return the tool to a diameter outside of the workpiece blank diameter after roughing. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
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 stud. 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 | |
Q206 Feed rate for plunging? Traversing speed of the tool in mm/min while moving to depth Input: 0...99999.999 or FAUTO, FMAX, FU, FZ | |
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...1.9999 or PREDEF | |
Q215 Machining operation (0/1/2)? Define the machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing Input: 0, 1, 2 | |
Q369 Finishing allowance for floor? Finishing allowance for the floor. This value has an incremental effect. Input: 0...99999.9999 | |
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 | |
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 |
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 258 POLYGON STUD ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 L X+50 Y+50 R0 FMAX M99 |