Cycle 19 WORKING PLANE (option 8)

Application

 
Machine

Refer to your machine manual.

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

raumw1
Schwenkw

Use Cycle 19 to define the position of the working plane—i.e. the position of the tool axis referenced to the machine coordinate system—by entering tilt angles. There are two ways to determine the position of the working plane:

  • Enter the position of the rotary axes directly.
  • Describe the position of the working plane using up to three rotations (spatial angles) of the machine-based coordinate system.
  • The required spatial angles can be calculated by cutting a perpendicular line through the tilted working plane and considering it from the axis around which you wish to tilt. With two spatial angles, every tool position in space can be defined exactly.

 
Tip

Note that the position of the tilted coordinate system, and therefore also all movements in the tilted system, are dependent on your description of the tilted plane.

If you program the position of the working plane via spatial angles, the control will calculate the required angle positions of the tilted axes automatically and will store these in the Q120 (A axis) to Q122 (C axis) parameters. If two solutions are possible, the control will choose the shorter path from the current position of the rotary axes.

The axes are always rotated in the same sequence for calculating the tilt of the plane: The control first rotates the A axis, then the B axis, and finally the C axis.

Cycle 19 becomes effective as soon as it has been defined in the NC program. As soon as you move an axis in the tilted system, the compensation for this specific axis will be activated. You must move all axes to activate compensation for all axes.

If you set the Program Run switch in the 3D ROT menu (Manual operation operating mode / Manual operation) application to active, the angular value entered in this menu is overwritten by Cycle 19 WORKING PLANE.

Notes

  • This cycle can be executed in the FUNCTION MODE MILL machining mode.
  • In combination with a radial facing slide kinematics model, this cycle can also be used in the FUNCTION MODE TURN machining mode.
  • The working plane is always tilted around the active datum.
  • If you use the Cycle 19 while M120 is active, the control automatically cancels the radius compensation, which also cancels the M120 function.

Notes on programming

  • Write the program as if the machining process was to be executed in a non-tilted plane.
  • If you call the cycle again for other angles, you do not need to reset the machining parameters.
 
Tip

Because nonprogrammed rotary axis values are interpreted as unchanged, you should always define all three spatial angles, even if one or more angles are at zero.

Notes about machine parameters

  • The machine manufacturer specifies whether the programmed angles are interpreted by the control as coordinates of the rotary axes (axis angles) or as angular components of a tilted plane (spatial angles).
  • In the machine parameter CfgDisplayCoordSys (no. 127501) the machine manufacturer defines the coordinate system in which the status display shows an active datum shift.

Cycle parameters

Help graphic

Parameter

raumw2

Rotary axis and angle?

Enter the axis of rotation together with the associated tilt angles. Program the rotary axes A, B and C using the action bar.

Input: –360.000...+360.000

If the control automatically positions the rotary axes, you can enter the following parameters:

Help graphic

Parameter

Feed rate? F=

Traverse speed of the rotary axis during automatic positioning

Input: 0...300000

Set-up clearance?

The control positions the tilting head in such a way that the position that results from the extension of the tool by the set-up clearance does not change relative to the workpiece. This value has an incremental effect.

Input: 0...999999999

Reset

To reset the tilt angles, redefine Cycle 19 WORKING PLANE. Enter an angular value of 0° for all rotary axes. Then, redefine Cycle 19 WORKING PLANE. Confirm the dialog prompt by pressing the NO ENT key. This disables the function.

Positioning the axes of rotation

 
Machine

Refer to your machine manual.

The machine manufacturer determines whether Cycle 19 positions the axes of rotation automatically or whether they need to be positioned manually in the NC program.

Manual positioning of rotary axes

If Cycle 19 does not position the rotary axes automatically, you need to position them in a separate L block following the cycle definition.

If you use axis angles, you can define the axis values right in the L block. For using spatial angles, program the Q parameters Q120 (A axis value), Q121 (B axis value) and Q122 (C axis value) according to Cycle 19.

 
Tip

For manual positioning, always use the rotary axis positions stored in Q parameters Q120 to Q122.

Avoid the use of functions such as M94 (modulo rotary axes) in order to prevent discrepancies between actual and nominal positions of the rotary axes for multiple calls.

Example

11 L Z+100 R0 FMAX

12 L X+25 Y+10 R0 FMAX

* - ...

; Define the spatial angles for calculating the compensation

13 CYCL DEF 19.0 WORKING PLANE

14 CYCL DEF 19.1 A+0 B+45 C+0

15 L A+Q120 C+Q122 R0 F1000

; Position the rotary axes by using values calculated by Cycle 19

16 L Z+80 R0 FMAX

; Activate compensation for the spindle axis

17 L X-8.5 Y-10 R0 FMAX

; Activate compensation for the working plane

Automatic positioning of rotary axes

If the rotary axes are positioned automatically in Cycle 19:

  • The control can position only closed-loop axes.
  • To position the tilted axes, you must enter a feed rate and a set-up clearance, in addition to the tilting angles, when defining the cycle
  • Use only preset tools (the full tool length must have been defined)
  • The position of the tool tip as referenced to the workpiece surface remains nearly unchanged after tilting.
  • The control performs tilting at the last programmed feed rate (the maximum feed rate depends on the complexity of the swivel head geometry or tilting table)

Example

11 L Z+100 R0 FMAX

12 L X+25 Y+10 R0 FMAX

* - ...

; Angle for calculating the compensation; define the feed rate and clearance

13 CYCL DEF 19.0 WORKING PLANE

14 CYCL DEF 19.1 A+0 B+45 C+0 F5000 ABST50

15 L Z+80 R0 FMAX

; Activate compensation for the spindle axis

16 L X-8.5 Y-10 R0 FMAX

; Activate compensation for the working plane

Position display in a tilted system

On activation of Cycle 19, the displayed positions (NOML and ACTL) and the datum indicated in the additional status display are referenced to the tilted coordinate system. This means that the position displayed immediately after cycle definition might not be the same as the coordinates of the last programmed position before Cycle 19.

Monitoring of the working space

The control monitors only those axes in the tilted coordinate system that are moved. Where applicable, the control displays an error message.

Positioning in a tilted coordinate system

With miscellaneous function M130, you can move the tool, while the coordinate system tilted, to positions that reference the non-tilted coordinate system.

With a tilted working plane, it is also possible to position the axes using straight-line blocks that reference the machine coordinate system (NC blocks with M91 or M92). Constraints:

  • Positioning is without length compensation.
  • Positioning is done without length compensation.
  • Tool radius compensation is not allowed.

Combining coordinate transformation cycles

When combining coordinate transformation cycles, always make sure the working plane is tilted about the active datum. You can program a datum shift before activating Cycle 19. In this case, you are shifting the machine-based coordinate system.

If you program a datum shift after the activation of Cycle 19 , you are shifting the tilted coordinate system.

Important: When resetting the cycles, reverse the sequence used for defining them:

  1. Activate datum shift
  2. Activate Tilt working plane
  3. Activate rotation

...

Workpiece machining

...

  1. Reset the rotation
  2. Reset Tilt working plane
  3. Reset the datum shift

Procedure for working with Cycle 19 WORKING PLANE

  1. Proceed as follows:
  2. Create the NC program
  3. Clamp the workpiece
  4. Set any presets
  5. Start the NC program
  1. Creating the NC program:
  2. Call the defined tool
  3. Retract in the spindle axis
  4. Position the axes of rotation
  5. Activate a datum shift if required
  6. Define Cycle 19 WORKING PLANE
  7. Position all principal axes (X, Y, Z) in order to activate the compensation
  8. Define Cycle 19 with different angles, if necessary
  9. Reset Cycle 19 by programming 0° for all rotary axes
  10. Redefine Cycle 19 in order to deactivate the working plane
  11. Reset datum shift if required.
  12. Position the tilt axes to the 0° position if required.

You can define the preset in the following ways:

  • Manually by touch-off
  • Controlled with a HEIDENHAIN 3-D touch probe
  • Automatically with a HEIDENHAIN 3-D touch probe

Touch Probe Cycles: Automatic Preset Measurement

Workpiece presetting with a touch probe