Cycle 275 TROCHOIDAL SLOT
ISO programming
G275
Application
In conjunction with Cycle 14 CONTOUR , 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 (#45 / #2-31-1)).
Adaptive Feed Control (AFC) (#45 / #2-31-1)
Depending on the cycle parameters you select, the following machining alternatives are available:
- Complete machining: Roughing, side finishing
- Only roughing
- Only side finishing
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 |
Cycle sequence
Roughing closed slots
In case of a closed slot, the contour description must always start with a straight-line block (L block).
- Following the positioning logic, the tool moves to the starting point of the contour description and moves to the first infeed depth in a reciprocating motion at the plunging angle defined in the tool table. Specify the plunging strategy with parameter Q366.
- The control roughs the slot in circular motions until the contour end point is reached. During the circular motion, the control moves the tool in the machining direction by a user-definable infeed (Q436). Define climb or up-cut of the circular motion in parameter Q351.
- At the contour end point, the control moves the tool to clearance height and returns it to the starting point of the contour description.
- This process is repeated until the programmed slot depth is reached.
Finishing closed slots
- If a finishing allowance has been defined, the control finishes the slot walls, in multiple infeeds, if so specified. Starting from the defined starting point, the control approaches the slot wall tangentially. Climb or up-cut milling is taken into consideration.
Roughing open slots
The contour description of an open slot must always start with an approach block (APPR).
- Following the positioning logic, the tool moves to the starting point of the machining operation as defined by the parameters in the APPR block and plunges vertically to the first plunging depth.
- The control roughs the slot in circular motions until the contour end point is reached. During the circular motion, the control moves the tool in the machining direction by a user-definable infeed (Q436). Define climb or up-cut of the circular motion in parameter Q351.
- At the contour end point, the control moves the tool to clearance height and returns it to the starting point of the contour description.
- This process is repeated until the programmed slot depth is reached.
Finishing open slots
- If a finishing allowance has been defined, the control finishes the slot walls (in multiple infeeds if specified). The control approaches the slot wall starting from the defined starting point of the APPR block. Climb or up-cut milling is taken into consideration.
Notes
- After the end of the cycle, position the tool with all coordinates of the working plane (e.g., L X+80 Y+0 R0 FMAX)
- Make sure to program an absolute position after the cycle; do not program an incremental traversing movement
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- The memory capacity for programming an SL cycle is limited. You can program up to 16384 contour elements in one SL cycle.
- In conjunction with Cycle 275, the control does not require Cycle 20 CONTOUR DATA.
- This cycle finishes Q369 ALLOWANCE FOR FLOOR with only one infeed. Parameter Q338 INFEED FOR FINISHING has no effect on Q369. Q338 is effective in finishing of Q368 ALLOWANCE FOR SIDE.
- The cycle considers the miscellaneous functions M109 and M110. During the inside and outside machining of circular arcs the control keeps the feed rate constant at the cutting edge for inside and outside radii.
Notes on programming
- The algebraic sign for the DEPTH cycle parameter determines the working direction. If you program DEPTH=0, the cycle will not be executed.
- If using Cycle 275 TROCHOIDAL SLOT, you may define only one contour subprogram in Cycle 14 CONTOUR.
- Define the center line of the slot with all available path functions in the contour subprogram.
- The starting point of a closed slot must not be located in a contour corner.
Cycle parameters
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. This value has an incremental effect. Maximum slot width for roughing: Twice the tool diameter Input: 0...99999.9999 | |
Q368 Finishing allowance for side? Finishing allowance in the machining plane which remains after roughing. 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? Infeed in the tool axis when finishing the lateral finishing allowance Q368. This value has an incremental effect. 0: Finishing in one infeed 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? (optional) Finishing allowance in depth which remains after roughing. This value has an incremental effect. Input: 0...99999.9999 | |
Q439 Feed rate reference (0-3)? (optional) 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.
Change the following contents as needed:
- Tools
- Cutting parameters
- Feed rates
- Clearance height or safe position
- Machine-specific positions (e.g., with M91)
- Paths of program calls
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 |