ISO programming
G275
G275
In conjunction with Cycle 14 KONTUR, this cycle enables you to completely machine open and closed slots or contour slots using trochoidal milling.
With trochoidal milling, large cutting depths and high cutting speeds can be combined as the equally distributed cutting forces prevent increased wear of the tool. When indexable inserts are used, the entire cutting length is exploited to increase the attainable chip volume per tooth. Moreover, trochoidal milling is easy on the machine mechanics. Enormous amounts of time can also be saved by combining this milling method with the integrated adaptive feed control AFC (option 45).
Adaptive Feed Control (AFC, option 45)
Depending on the cycle parameters you select, the following machining alternatives are available:
0 BEGIN CYC275 MM |
---|
... |
12 CYCL DEF 14 CONTOUR |
... |
13 CYCL DEF 275 TROCHOIDAL SLOT |
... |
14 CYCL CALL M3 |
... |
50 L Z+250 R0 FMAX M2 |
51 LBL 10 |
... |
55 LBL 0 |
... |
99 END PGM CYC275 MM |
Roughing closed slots
In case of a closed slot, the contour description must always start with a straight-line block (L block).
Finishing closed slots
Roughing open slots
The contour description of an open slot must always start with an approach block (APPR).
Finishing open slots
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 | |
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 | |
Q436 Feed per revolution? Value by which the control moves the tool in the machining direction per revolution. This value has an absolute effect. Input: 0...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 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 | |
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 | |
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 | |
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 | |
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 = No function 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 Input: 0, 1, 2 or PREDEF | |
Q369 Finishing allowance for floor? Finishing allowance for the floor. This value has an incremental effect. Input: 0...99999.9999 | |
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 275 TROCHOIDAL SLOT ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 CYCL CALL |