Using a facing head with FACING HEAD POS (#50 / #4-03-1)
Application
A facing head, also called facing slide, allows you to perform almost all turning operations with fewer different tools. The position of the facing head is programmable in the X direction. On the facing head, you mount, for example, a longitudinal turning tool that you call with a TOOL CALL block.
Related topics
- Machining with parallel axes U, V and W
Requirements
- Software option Turning (#50 / #4-03-1)
- Control prepared by the machine manufacturer
The machine manufacturer must take the facing head into account in the kinematics.
- Kinematics with facing head activated
- Workpiece datum in the working plane is at the center of the rotationally symmetrical contour
With a facing head, the workpiece datum must not be in the center of the rotary table, because the tool spindle rotates.
Description of function
Refer to your machine manual.
The machine manufacturer can provide customized cycles for working with a facing head. The standard functionality is described below.
The facing head is defined as a turning tool.
Turning tool table toolturn.trn (#50 / #4-03-1)
Please note for tool calls:
- TOOL CALL block without tool axis
- Cutting speed and spindle speed with TURNDATA SPIN
- Switch the spindle on with M3 or M4
Machining also works with a tilted working plane and on workpieces that are not rotationally symmetric.
If you move with the facing head without the FACING HEAD POS function, you must program the motions of the facing head with the U axis (e.g., in the Manual operation application). If the FACING HEAD POS function is active, program the facing head with the X axis.
When you activate the facing head, the control automatically positions itself at the workpiece datum in X and Y. To avoid collisions, you can define a safe height using the HEIGHT syntax element.
The facing head is deactivated with the FUNCTION FACING HEAD function.
Input
Activating the facing head
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 FACING HEAD POS HEIGHT+100 FMAX | ; Activate facing head and move with rapid traverse to safe height Z+100 |
To navigate to this function:
Insert NC function All functions Special functions Turning functions Facing slide FACING HEAD POS
The NC function includes the following syntax elements:
Syntax element | Meaning |
---|---|
FACING HEAD POS | Activate the syntax initiator for the facing head |
HEIGHT | Safe height in the tool axis Optional syntax element |
F or FMAX | Approach safe height with defined feed rate or rapid traverse Optional syntax element |
M | Additional function Optional syntax element |
Deactivating the facing head
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 FUNCTION FACING HEAD OFF | ; Deactivate facing head |
To navigate to this function:
Insert NC function All functions Special functions Turning functions Facing slide FUNCTION FACING HEAD OFF
The NC function includes the following syntax elements:
Syntax element | Meaning |
---|---|
FUNCTION FACING HEAD OFF | Deactivate the syntax initiator for the facing head |
Notes
- Position the facing head at its home position while the FACING HEAD POS function is active
- Retract the facing head while the FACING HEAD POS function is active
- In the Manual operation operating mode, move the facing head with the U axis key.
- As the Tilt working plane function can be used, pay attention to the 3D ROT status
- To set a spindle-speed limitation, you can use the NMAX value from the tool table as well as the SMAX value from FUNCTION TURNDATA SPIN.
- The following constraints apply to the use of a facing head:
- Miscellaneous functions M91 and M92 cannot be used
- Retraction with M140 is not possible
- TCPM or M128 are not possible (#9 / #4-01-1)
- DCM collision monitoring cannot be used (#40 / #5-03-1)
- Cycles 800, 801, and 880 cannot be used
- Cycles 286 and 287 cannot be used (#157 / #4-05-1)
- If you are using the facing head in the tilted working plane, please note the following:
- The control calculates the tilted working plane as in milling mode. The COORD ROT and TABLE ROT functions, as well as SYM (SEQ), reference the XY plane.
- HEIDENHAIN recommends selecting the TURN positioning behavior. The MOVE positioning behavior is not the best option in combination with the facing head.
Notes about machine parameters
The machine manufacturer uses the optional machine parameter presetToAlignAxis (no. 300203) to define for each axis how the control is to interpret offset values. If FACING HEAD POS is used, the machine parameter applies to the parallel axis (U axis) only (U_OFFS).
Basic transformation and offset
- If the machine parameter has not been defined or has been set to FALSE, the control does not take the offset into account during machining.
- If the machine parameter axis has been set to TRUE, the offset can be used to compensate for a facing head offset. If you are using a facing head with multiple tool clamp options, set the offset for the current clamping position. This ensures that you can run NC programs independent of the tool clamping position.