Cycle 815 CONTOUR-PAR. TURNING
ISO programming
G815
Application
Refer to your machine manual.
This function must be enabled and adapted by the machine manufacturer.
This cycle enables you to execute turning of workpieces with any turning contours. The contour description is in a subprogram.
You can use the cycle either for roughing, finishing or complete machining. Turning with roughing is contour-parallel.
The cycle can be used for inside and outside machining. If the coordinate of the contour starting point is larger than that of the contour end point, the cycle runs outside machining. If the coordinate of the contour starting point is less than that of the contour end point, the cycle runs inside machining.
Roughing cycle sequence
The control uses the tool position as cycle starting point when the cycle is called. If the Z coordinate of the starting point is less than the contour starting point, the control positions the tool in the Z coordinate to set-up clearance and begins the cycle there.
- The control performs a paraxial infeed movement at rapid traverse. The control calculates the infeed value based on Q463 Maximum cutting depth.
- The control machines the area between the starting position and end point. The cut is performed in contour-parallel mode at the defined feed rate Q478.
- The control returns the tool at the defined feed rate back to the starting position in the X coordinate.
- The control returns the tool at rapid traverse to the beginning of cut.
- The control repeats this procedure (steps 1 to 4) until the contour is completed.
- The control returns the tool at rapid traverse to the cycle starting point.
Finishing cycle sequence
If the Z coordinate of the starting point is less than the contour starting point, the control positions the tool in the Z coordinate to set-up clearance and begins the cycle there.
- The infeed movement is performed at rapid traverse.
- The control finishes the contour of the finished part (contour starting point to contour end point) at the defined feed rate Q505.
- The control retracts the tool at the defined feed rate to the set-up clearance.
- The control returns the tool at rapid traverse to the cycle starting point.
Notes
- This cycle can be executed only in the FUNCTION MODE TURN machining mode.
- The tool position at cycle call (cycle start point) influences the area to be machined.
- The control takes the cutting geometry of the tool into account to prevent damage to contour elements. If it is not possible to machine the entire workpiece with the active tool, the control will display a warning.
- Also refer to the fundamentals of the turning cycles.
Notes on programming
- Program a positioning block to a safe position with radius compensation R0 before the cycle call.
- Before programming the cycle call, make sure to program Cycle 14 CONTOUR or SEL CONTOUR to be able to define the subprograms.
- If you use local QL Q parameters in a contour subprogram, you must also assign or calculate these in the contour subprogram.
- Finishing the contour requires programming tool radius compensation RL or RR in the contour description.
Cycle parameters
Help graphic | Parameter |
---|---|
Q215 Machining operation (0/1/2/3)? Define extent of machining: 0: Roughing and finishing 1: Only roughing 2: Only finishing to final dimension 3: Only finishing to oversize Input: 0, 1, 2, 3 | |
Q460 Set-up clearance? Distance for retraction and prepositioning. This value has an incremental effect. Input: 0...999.999 | |
Q485 Allowance for workpiece blank? Contour-parallel oversize on the defined contour. This value has an incremental effect. Input: 0...99.999 | |
Q486 Type of cut lines (=0/1)? Define the type of cutting lines: 0: Cuts with consistent chip cross section 1: Equidistance cut distribution Input: 0, 1 | |
Q499 Reverse the contour (0-2)? Define the machining direction of the contour: 0: Contour is executed in the programmed direction 1: Contour is executed in the direction opposite to the programmed direction 2: Contour is executed in the direction opposite to the programmed direction; the position of the tool is also adjusted Input: 0, 1, 2 | |
Q463 Maximum cutting depth? Maximum infeed (radius value) in the radial direction. The infeed is distributed evenly to avoid abrasive cuts. Input: 0...99.999 | |
Q478 Roughing feed rate? Feed rate during roughing. If M136 has been programmed, the value is interpreted by the control in millimeters per revolution; without M136, in millimeters per minute. Input: 0...99999.999 or FAUTO | |
Q483 Oversize for diameter? Diameter oversize on the defined contour. This value has an incremental effect. Input: 0...99.999 | |
Q484 Oversize in Z? Oversize of the defined contour in the axial direction. This value has an incremental effect. Input: 0...99.999 | |
Q505 Finishing feed rate? Feed rate during finishing. If M136 has been programmed, the value is interpreted by the control in millimeters per revolution; without M136, in millimeters per minute. Input: 0...99999.999 or FAUTO |
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 815 CONTOUR-PAR. TURNING ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 L X+75 Y+0 Z+2 FMAX M303 | ||
13 CYCL CALL |