Cycle 882 SIMULTANEOUS ROUGHING FOR TURNING (#158 / #4-03-2)
ISO programming
G882
Application
Refer to your machine manual.
This function must be enabled and adapted by the machine manufacturer.
In Cycle 882 SIMULTANEOUS ROUGHING FOR TURNING, the defined contour area is roughed simultaneously in several steps using a movement that includes at least 3 axes (two linear axes and one rotary axis). This allows machining of complex contours with a single tool. During machining, the cycle continuously adjusts the tool angle of inclination based on the following criteria:
- Avoiding collisions between the workpiece, the tool, and the tool carrier
- The tooth does not suffer single-spot wear
- Undercuts are possible
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
Roughing cycle sequence
- The cycle positions the tool at the cycle start position (tool position when the cycle is called), taking the first tool angle of inclination into account. Then, the tool moves to set-up clearance. If the angle of inclination cannot be achieved at the cycle start position, the control first moves the tool to set-up clearance and from there tilts it using the first tool angle of inclination.
- The tool moves to the plunging depth Q519. The profile infeed may be exceeded for a short time up to the value of Q463 MAX. CUTTING DEPTH (for example, when machining a corner).
- The contour is roughed simultaneously using the roughing feed-rate in Q478. If you define the plunging feed rate Q488 in the cycle, it will be effective for the plunging elements. Machining depends on the following input parameters:
- Q590: MACHINING MODE
- Q591: MACHINING SEQUENCE
- Q389: UNI.- BIDIRECTIONAL
- After each infeed, the control lifts the tool in rapid traverse by the set-up clearance value.
- The control repeats steps 2 to 4 until the contour has been machined completely.
- The control retracts the tool at the machining feed rate by the set-up clearance value and then moves it with rapid traverse to the starting position (first in the X axis and then in the Z axis direction)
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
- Prove-out the NC program in Program Run in Single Block mode
- Limit the machining area
- Run a simulation to verify the sequence and the contour
- This cycle can be executed only in the FUNCTION MODE TURN machining mode.
- If you programmed M136 before the cycle call, the control interprets the feed rate in millimeters per revolution.
- 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.
- If it is not possible to machine a particular contour area using this cycle, the control tries to divide the contour area into subareas that can be reached so as to machine them individually.
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.
- 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.
- The cycle requires a radius compensation (RL/RR) in its contour description.
- If you use local QL Q parameters in a contour subprogram, you must also assign or calculate these in the contour subprogram.
- 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.
- Define a value in Q463 MAX. CUTTING DEPTH relative to the cutting edge because, depending on the tool inclination, the infeed from Q519 may be temporarily exceeded. Use this parameter to limit the extent to which the infeed may be exceeded.
Cycle parameters
Help graphic | Parameter |
---|---|
Q460 Set-up clearance? Retraction before and after a cut. And distance for the pre-positioning. 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 | |
Q478 Roughing feed rate? Feed rate during roughing in millimeters per minute Input: 0...99999.999 or FAUTO | |
Q488 Feed rate for plunging Feed rate in millimeters per minute for plunging. This input value is optional. If you do not program the feed rate for plunging, the roughing feed rate Q478 will apply. 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 | |
Q567 Finishing allowance of contour? Contour-parallel oversize that will remain after roughing. This value has an incremental effect. Input: -9...99.999 | |
Q519 Infeed on contour? Axial, radial and contour-parallel infeed (per cut). Enter a value greater than 0. This value has an incremental effect. Input: 0.001...99.999 | |
Q463 Maximum cutting depth? Limit of the maximum infeed relative to the cutting edge. Depending on the tool angle of inclination, the control may temporarily exceed the Q519 INFEED (for example, when machining a corner). Use this optional parameter to limit the extent by which the infeed may be exceeded. If you define the value 0, the maximum infeed is two thirds of the length of the cutting edge. Input: 0...99.999 | |
Q590 Machining mode (0/1/2/3/4/5)? Defining the direction of machining: 0: Automatic; the control automatically combines transverse and longitudinal machining. 1: Longitudinal turning (outside) 2: Face turning (front face) 3: Longitudinal turning (inside) 4: Face turning (chuck) 5: Contour-parallel Input: 0, 1, 2, 3, 4, 5 | |
Q591 Machining sequence (0/1)? Define the machining sequence after which the control executes the contour: 0: Machining occurs in segments. The sequence is selected in such a way that the center of gravity of the workpiece is shifted towards the chuck as soon as possible. 1: The workpiece is machined paraxially. The sequence is selected in such a way that the moment of inertia of the workpiece decreases as soon as possible. Input: 0, 1 | |
Q389 Machining strategy (0/1)? Definite the cutting direction: 0: Unidirectional; every cut is made in the direction of the contour. The direction of the contour depends on Q499 1: Bidirectional; cuts are made against the direction of the contour. The cycle determines the best direction for each following step. Input: 0, 1 |
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 882 SIMULTANEOUS ROUGHING FOR TURNING ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 L X+58 Y+0 FMAX M303 | ||
13 L Z+50 FMAX | ||
14 CYCL CALL |