ISO programming
G815
G815
Refer to your machine manual.
This function must be enabled and adapted by the machine manufacturer.
This cycle enables you to run 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.
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.
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.
Fundamentals of turning cycles
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? Freed 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.
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 |