Taking rotary axes into account during machining operations with M138
Application
With M138 you define which rotary axes the control takes into account during the calculation and positioning of spatial angles. The control excludes any axes that were not defined. That way you can reduce the number of tilting possibilities and thus avoid error messages, for example on machines with three rotary axes.
M138 is in effect in combination with the following functions:
- M128 (#9 / #4-01-1)
Compensating the tool angle of inclination automatically with M128 (#9 / #4-01-1)
- FUNCTION TCPM (#9 / #4-01-1)
Compensating the tool angle of inclination with FUNCTION TCPM (#9 / #4-01-1)
- PLANE functions (#8 / #1-01-1)
Tilting the working plane with PLANE functions (#8 / #1-01-1)
- Cycle 19 WORKING PLANE (#8 / #1-01-1)
Description of function
Effect
M138 takes effect at the start of the block.
In order to reset M138, program M138 without entering any rotary axes.
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+100 R0 FMAX M138 A C | ; Define that axes A and C should be taken into account |
12 PLANE SPATIAL SPA+0 SPB+90 SPC+0 TURN FMAX | ; Tilt spatial angle SPB by 90° |
On a six-axis machine with A, B, and C rotary axes you must exclude one rotary axis for spatial angle operations; otherwise too many combinations are possible.
With M138 A C the control calculates the axis position when tilting with spatial angles only in the A and C axes. The B axis is excluded. Therefore, in NC block 12 the control positions the spatial angle SPB+90 with the A and C axes.
Without M138 there are too many possibilities for tilting. The control interrupts the machining process and issues an error message.
Input
If you define M138, the control continues the dialog and prompts you for the rotary axes to be taken into account.
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+100 R0 FMAX M138 C | ; Define that the C axis should be taken into account |
Notes
- With M138 the control excludes the rotary axes only during the calculation and positioning of spatial angles. A rotary axis that has been excluded with M138 can nevertheless be moved in a positioning block. Please note that in this case the control does not execute any compensations.
- The TNC7 basic can move up to four axes simultaneously. If an NC block commands movement of more than four axes, the control displays an error message.If the axis position does not change, you can nevertheless program more than four axes.
- In the optional machine parameter parAxComp (no. 300205) the machine manufacturer defines whether the control includes the position of the excluded axis when calculating the kinematics.