ISO programming
G883
G883
Refer to your machine manual.
This function must be enabled and adapted by the machine manufacturer.
The cycle is machine-dependent.
You can use this cycle to machine complex contours that are only accessible with different inclinations. When machining with this cycle, the inclination between tool and workpiece changes. This results in machining operations with at least 3 axes (two linear axes and one rotary axis).
The cycle monitors the workpiece contour with respect to the tool and the tool carrier. The cycle avoids unnecessary tilting movements in order to machine optimum surfaces.
If you want to force tilting movements, you can define inclination angles at the beginning and at the end of the contour. Even if simple contours have to be machined, you can use a large area of the indexable insert to achieve longer tool life.
You can execute this cycle with FreeTurn tools. This method allows you to perform the most common turning operations with just one tool. Machining times can be reduced through the flexible tool because fewer tool changes occur.
Requirements:
The NC program remains unchanged except for the calling of the FreeTurn cutting edges, see Example: Turning with a FreeTurn tool
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.
Help graphic | Parameter |
---|---|
Q460 Set-up clearance? Distance for retraction and prepositioning. This value has an incremental effect. Input: 0...999.999 | |
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 | |
Q558 Extensn. angle at contour start? Angle in the WPL-CS, by which the cycle extends the contour up to the workpiece blank at the programmed starting point. This angle is used to prevent damage to the workpiece blank. Input: -180...+180 | |
Q559 Extension angle at contour end? Angle in WPL CS by which the cycle extends the contour at the programmed end point up to the workpiece blank. This angle is used to prevent damage to the workpiece blank. Input: -180...+180 | |
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 | |
Q556 Minimum angle of inclination? Smallest possible permitted angle of inclination between the tool and workpiece relative to the Z axis. Input: -180...+180 | |
Q557 Maximum angle of inclination? Largest possible angle of inclination between the tool and workpiece relative to the Z axis. Input: -180...+180 | |
Q555 Stepping angle for calculation? Cutting width for the calculation of possible solutions Input: 0.5...9.99 | |
Q537 Inclin. angle (0=N/1=J/2=S/3=E)? Define whether an inclination angle is active: 0: No inclination angle active 1: Inclination angle active 2: Inclination angle at contour start active 3: Inclination angle at contour end active Input: 0, 1, 2, 3 | |
Q538 Inclin. angle at contour start? Inclination angle at the beginning of the programmed contour (WPL-CS) Input: -180...+180 | |
Q539 Inclinatn. angle at contour end? Inclination angle at the end of the programmed contour (WPL-CS) Input: -180...+180 | |
Q565 Finishing allowance in diameter Diameter oversize that remains on the contour after finishing. This value has an incremental effect. Input: -9...99.999 | |
Q566 Finishing allowance in Z? Oversize on the defined contour in the axial direction that remains on the contour after finishing. This value has an incremental effect. Input: -9...99.999 | |
Q567 Finishing allowance of contour? Contour-parallel oversize on the defined contour that remains after finishing. This value has an incremental effect. Input: -9...99.999 |
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 883 TURNING SIMULTANEOUS FINISHING ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 L X+58 Y+0 FMAX M303 | ||
13 L Z+50 FMAX | ||
14 CYCL CALL |