Cycle 291 COUPLG.TURNG.INTERP. (option 96)

ISO programming

G291

Application

 
Machine

Refer to your machine manual.

This function must be enabled and adapted by the machine manufacturer.

Cyc291_1

Cycle 291 COUPLG.TURNG.INTERP. couples the tool spindle to the position of the linear axes, or cancels this spindle coupling. With interpolation turning, the cutting edge is oriented to the center of a circle. The center of rotation is defined in the cycle by entering the coordinates Q216 and Q217.

Cycle sequence

  1. Q560=1:
  2. The control first performs a spindle stop (M5).
  3. The control orients the tool spindle to the specified center of rotation. The specified angle for spindle orientation Q336 is taken into account. If an "ORI" value is given in the tool table, it is also taken into account.
  4. The tool spindle is now coupled to the position of the linear axes. The spindle follows the nominal position of the reference axes.
  5. To terminate the cycle, the coupling must be deactivated by the operator. (With Cycle 291 or end of program/internal stop.)
  1. Q560=0:
  2. The control deactivates the spindle coupling.
  3. The tool spindle is no longer coupled to the position of the linear axes.
  4. The control ends machining with Cycle 291 COUPLG.TURNG.INTERP.
  5. If Q560=0, parameters Q336, Q216, Q217 are not relevant

Notes

 
Machine

This cycle is effective only for machines with servo-controlled spindle.

Your control might monitor the tool to ensure that no positioning movements at feed rate are performed while spindle rotation is off. Contact the machine manufacturer for further information.

  • This cycle can only be executed in the FUNCTION MODE MILL machining mode.
  • Cycle 291 is CALL-active.
  • This cycle can also be used in a tilted working plane.
  • Remember that the axis angle must be equal to the tilt angle before the cycle call! Only then can the axis be correctly coupled.
  • If Cycle 8 MIRRORING is active, the control does not execute the interpolation turning cycle.
  • If Cycle 26 AXIS-SPECIFIC SCALING is active, and the scaling factor for the axis does not equal 1, the control does not perform the cycle for interpolation turning.

Notes on programming

  • Programming of M3/M4 is not required. To describe the circular motions of the linear axes, you can, for example, use CC and C blocks.
  • When programming, remember that neither the spindle center nor the indexable insert must be moved into the center of the turning contour.
  • Program outside contours with a radius greater than 0.
  • Program inside contours with a radius greater than the tool radius.
  • In order to attain high contouring speeds for your machine, define a large tolerance with Cycle 32 before calling the cycle. Program Cycle 32 with HSC filter=1.
  • After defining Cycle 291 and CYCL CALL, program the operation you wish to perform. To describe the circular motions of the linear axes, you can use linear or polar coordinates, for example.
  • Example: Interpolation turning with Cycle 291

Note regarding machine parameters

  • In the machine parameter mStrobeOrient (no. 201005), the machine manufacturer defines the M function for spindle orientation.
    • If the value is > 0, the control executes this M number to perform the oriented spindle stop (PLC function defined by the machine manufacturer). The control waits until the oriented spindle stop has been completed.
    • If you enter –1, the control will perform the oriented spindle stop.
    • If you enter 0, no action will be taken.

    The control will, under no circumstances, output M5 before.

Cycle parameters

Help graphic

Parameter

Q560 Spindle coupling (0=off, 1=on)?

Define whether the tool spindle will be coupled to the position of the linear axes. If spindle coupling is active, the tool's cutting edge is oriented to the center of rotation.

0: Spindle coupling off

1: Spindle coupling on

Input: 0, 1

Q336 Angle for spindle orientation?

The control orients the tool to this angle before starting the machining operation. If you work with a milling tool, enter the angle in such a way that one cutting edge is turned towards the center of rotation.

If you work with a turning tool, and have defined the value "ORI" in the turning tool table (toolturn.trn), then it is taken into account for the spindle orientation.

Input: 0...360

Defining the tool

291-04

Q216 Center in 1st axis?

Center of rotation in the main axis of the working plane

Absolute input: –99999.9999...99999.9999

Q217 Center in 2nd axis?

Center of rotation in the secondary axis of the working plane

Input: –99999.9999...+99999.9999

Q561 Convert turning tool (0/1)

Only relevant if you define the turning tool in the turning tool table (toolturn.trn). This parameter allows you to decide whether the value XL of the turning tool will be interpreted as radius R of a milling tool.

0: No change; the turning tool is interpreted as described in the turning tool table (toolturn.trn). In this case, you must not use the radius compensation RR or RL. Furthermore, you must describe the movement of the path of the tool center point TCP without spindle coupling when programming. This kind of programming is much more complicated.

1: The value XL from the turning tool table (toolturn.trn) is interpreted as a radius R of a milling tool table. This makes it possible to use radius compensation RR or RL when programming your contour. This kind of programming is recommended.

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.

 
Tip

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.

Example

11 CYCL DEF 291 COUPLG.TURNG.INTERP. ~

Q560=+0

;SPINDLE COUPLING ~

Q336=+0

;ANGLE OF SPINDLE ~

Q216=+50

;CENTER IN 1ST AXIS ~

Q217=+50

;CENTER IN 2ND AXIS ~

Q561=+0

;CONVERT FROM TURNING TOOL

Defining the tool

Overview

Depending on the entry for parameter Q560 you can either activate (Q560=1) or deactivate (Q560=0) the COUPLG.TURNG.INTERP. cycle.

Spindle coupling off, Q560=0

The tool spindle is not coupled to the position of the linear axes.

 
Tip

Q560=0: Disable the COUPLG.TURNG.INTERP. cycle!

Spindle coupling on, Q560=1

A turning operation is executed with the tool spindle coupled to the position of the linear axes. If you set the parameter Q560=1, there are different possibilities to define the tool in the tool table. This section describes the different possibilities:

  • Define a turning tool in the tool table (tool.t) as a milling tool
  • Define a milling tool in the tool table (tool.t) as a milling tool (for subsequent use as a turning tool)
  • Define a turning tool in the turning tool table (toolturn.trn)

These three possibilities of defining the tool are described in more detail below:

  • Define a turning tool in the tool table (tool.t) as a milling tool
  • If you are working without option 50, define your turning tool as a milling cutter in the tool table (tool.t). In this case, the following data from the tool table are taken into account (including delta values): length (L), radius (R), and corner radius (R2). The geometry data of the turning tool are converted to the data of a milling cutter. Align your turning tool to the spindle center. Specify this spindle orientation angle in parameter Q336 of the cycle. For outside machining, the spindle orientation equals the value in Q336, and for inside machining, the spindle orientation equals Q336+180.

     
    Notice
    Danger of collision!
    Collision may occur between the tool holder and workpiece during inside machining. The tool holder is not monitored. If the tool holder results in a larger rotational diameter than the cutter does, there is a danger of collision.
    1. Select the tool holder to ensure that it does not result in a larger rotational diameter than the cutter does
  • Define a milling tool in the tool table (tool.t) as a milling tool (for subsequent use as a turning tool)
  • You can perform interpolation turning with a milling tool. In this case, the following data from the tool table are taken into account (including delta values): length (L), radius (R), and corner radius (R2). Align one cutting edge of your milling cutter to the spindle center. Specify this angle in parameter Q336. For outside machining, the spindle orientation equals the value in Q336, and for inside machining, the spindle orientation equals Q336+180.

  • Define a turning tool in the turning tool table (toolturn.trn)
  • If you are working with option 50, you can define your turning tool in the turning tool table (toolturn.trn). In this case, the orientation of the spindle to the center of rotation takes place under consideration of tool-specific data, such as the type of machining (TO in the turning tool table), the orientation angle (ORI in the turning tool table), parameter Q336, and parameter Q561.

     
    Tip
    • Programming and operating notes:
    • If you define the turning tool in the turning tool table (toolturn.trn), we recommend working with parameter Q561=1. This way, you convert the data of the turning tool into the data of the milling tool, thus greatly facilitating your programming effort. With Q561=1 you can use radius compensation RR and RL when programming. (However, if you program Q561=0, then you cannot use radius compensation RR and RL when describing your contour. Additionally, you must program the movement of the tool center path TCP without spindle coupling. This kind of programming is much more complicated!)
      • If you programmed parameter Q561=1, you must program the following in order to conclude the interpolation turning machining operation:
      • R0, cancels radius compensation
      • Cycle 291 with parameters Q560=0 and Q561=0, deactivates spindle coupling
      • CYCL CALL, for calling Cycle 291
      • TOOL CALL overrides the conversion of parameter Q561
      • If you programmed parameter Q561=1, you may only use the following types of tools:
      • TYPE: ROUGH, FINISH, BUTTON with the machining directions TO: 1 or 8, XL>=0
      • TYPE: ROUGH, FINISH, BUTTON with the machining directions TO: 7: XL<=0

    The spindle orientation is calculated as follows:

    Machining

    TO

    Spindle orientation

    Interpolation turning, outside

    1

    ORI + Q336

    Interpolation turning, inside

    7

    ORI + Q336 + 180

    Interpolation turning, outside

    7

    ORI + Q336 + 180

    Interpolation turning, inside

    1

    ORI + Q336

    Interpolation turning, outside

    8

    ORI + Q336

    Interpolation turning, inside

    8

    ORI + Q336

    • You can use the following tool types for interpolation turning:
    • TYPE: ROUGH, with the machining directions TO: 1, 7, 8
    • TYPE: FINISH, with the machining directions TO: 1, 7, 8
    • TYPE: BUTTON, with the machining directions TO: 1, 7, 8
    • The following tool types cannot be used for interpolation turning:
    • TYPE: ROUGH, with the machining directions TO: 2 to 6
    • TYPE: FINISH, with the machining directions TO: 2 to 6
    • TYPE: BUTTON, with the machining directions TO: 2 to 6
    • TYPE: RECESS
    • TYPE: RECTURN
    • TYPE: THREAD