With M118 the control activates handwheel superimpositioning. You can then perform manual corrections by handwheel during program run.
Application
Related topics
- Handwheel superimpositioning with global program settings GPS (option 44)
Requirements
- Handwheel
- Software option 21: Advanced Functions (set 3)
Description of function
Effect
M118 takes effect at the start of the block.
In order to reset M118, program M118 without entering any axes.
Canceling a program also resets handwheel superimpositioning.
Application example
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 L Z+0 R0 F500 | ; Move in the tool axis |
12 L X+200 R0 F250 M118 Z1 | ; Move in the working plane with active handwheel superimpositioning of no more than ±1 mm in the Z axis |
In the first NC block the control positions the tool in the tool axis.
In NC block 12 the control activates handwheel superimpositioning at the start of the block with a maximum traverse range of ±1 mm in the Z axis.
Then the control performs the traverse movement in the working plane. During this traverse movement you can use the handwheel for continuous motion of the tool in the Z axis by up to ±1 mm. This way you can, for example, rework a workpiece that has been reclamped but that cannot be probed due to its free-form surface.
Input
If you define M118, the control continues the dialog and prompts you for the axes and the maximum permissible superimpositioning value. For linear axes you define the value in millimeters and for rotary axes in degrees.
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.
21 L X+0 Y+38.5 RL F125 M118 X1 Y1 | ; Move in the working plane with active handwheel superimpositioning of no more than ±1 mm in the X and Y axes |
Notes
Refer to your machine manual.
Your machine manufacturer must have prepared the control for this function.
- By default M118 is in effect in the machine coordinate system M-CS.
- On the POS HR tab of the Status workspace the control shows the active coordinate system in which handwheel superimpositioning is in effect, as well as the maximum possible traverse values of the respective axes.
- The handwheel superimpositioning function with M118 in combination with dynamic collision monitoring (DCM, option 40) is possible only at a standstill.
- Handwheel superimpositioning is also effective in the MDI application.
- If you want to use M118 with clamped axes, you must unclamp them first.
If you activate the handwheel superimpositioning switch in the GPS (option 44) workspace, handwheel superimpositioning is active in the last selected coordinate system.
Global Program Settings (GPS, option 44)
To be able to use M118 without restrictions, you have to deactivate DCM (option 40) or activate a kinematics model without collision objects.
Dynamic Collision Monitoring (DCM, option 40)
Notes in conjunction with the virtual tool axis VT (option 44)
Refer to your machine manual.
Your machine manufacturer must have prepared the control for this function.
- On machines with head rotation axes, you can choose for inclined machining whether superimpositioning should be in effect in the Z axis or along the virtual tool axis VT.
- In the machine parameter selectAxes (no. 126203) the machine manufacturer defines the assignment of axis keys on the handwheel.
When using an HR 5xx handwheel, you can assign the virtual axis to the orange VI axis key, if desired.