Cycle 883 TURNING SIMULTANEOUS FINISHING (#158 / #4-03-2)
ISO programming
G883
Application
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 three 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.
Execution with a FreeTurn tool
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:
- This function must be adapted by your machine manufacturer.
- You must properly define the tool.
The NC program remains unchanged except for the calling of the FreeTurn cutting edges, see Example: Turning with a FreeTurn tool
Finishing 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 moves the tool to the set-up clearance Q460. The movement is performed at rapid traverse.
- If programmed, the tool traverses to the inclination angle that was calculated by the control based on the minimum and maximum inclination angles you have defined.
- The control finishes the contour of the finished part (contour starting point to contour end point) simultaneously 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
- Run a simulation to verify the sequence and the contour
- Slowly prove-out the NC program
- Move the tool to a safe position in the X and Z axes.
- When clamping, take both the tool angle of inclination and the departure movement into account
- This cycle can be executed only in the FUNCTION MODE TURN machining mode.
- Based on the programmed parameters, the control calculates only one collision-free path.
- Software limit switches limit the possible inclination angles Q556 and Q557. If the software limit switches are deactivated in the Editor operating mode in the Simulation workspace, the simulation and the subsequent machining may be different.
- The cycle calculates a collision-free path. For this purpose, it only uses the 2D contour of the tool holder without considering the Y axis depth.
Notes on programming
- Before programming the cycle call, make sure to program Cycle 14 CONTOUR or SEL CONTOUR to be able to define the subprograms.
- Move the tool to a safe position before the cycle call.
- The cycle requires a radius compensation (RL/RR) in its contour description.
- Prior to the cycle call, you must program FUNCTION TCPM. HEIDENHAIN recommends programming the tool reference point REFPNT TIP-CENTER in FUNCTION TCPM. Use FUNCTION TCPM with the selection REFPNT TIP-CENTER to activate the virtual tool tip.
- If you use local QL Q parameters in a contour subprogram, you must also assign or calculate these in the contour subprogram.
- Please note: The smaller the resolution in cycle parameter Q555 is, the easier will it be to find a solution even in complex situations. The drawback is that the calculation will take more time.
- For determining the inclination angle, the cycle requires the definition of a tool holder. For this purpose, assign a tool holder to the tool in the KINEMATIC column of the tool table.
- Please note that cycle parameters Q565 (Finishing allowance in diameter) and Q566 (Finishing allowance in Z) cannot be combined with Q567 (Finishing allowance of contour)!
Cycle parameters
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.
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 883 TURNING SIMULTANEOUS FINISHING ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 L X+58 Y+0 FMAX M303 | ||
13 L Z+50 FMAX | ||
14 CYCL CALL |