You can combine the turning operation with function M128 or FUNCTION TCPM and REFPNT TIP-CENTER. This enables you to manufacture contours in one cut, for which you have to change the inclination angle (simultaneous machining).
Application
Related topics
- Cycles for simultaneous turning (option 158)
- Miscellaneous function M128 (option 9)
- FUNCTION TCPM (option 9)
Cycle 882 SIMULTANEOUS ROUGHING FOR TURNING (option158)
Automatically compensating for tool inclination with M128 (option 9)
Compensating for the tool angle of inclination with FUNCTION TCPM (option 9)
Requirements
- Machine with at least two rotary axes
- Combined milling/turning (software option 50)
- Advanced Functions Set 2 (software option 9)
Description of function
The simultaneous turning contour is a turning contour for which a rotary axis whose inclination does not violate the contour can be programmed on CP polar circles and L linear blocks. Collisions with lateral cutting edges or holders are not prevented. This makes it possible to finish contours with one tool in a continuous movement, even though different sections of the contour are accessible only in different tool inclinations.
In the NC program you define how the rotary axis has to be inclined to reach the different contour parts without collisions.
Use the cutter radius oversize DRS to leave an equidistant oversize on the contour.
Use FUNCTION TCPM and REFPNT TIP-CENTER to measure the theoretical tool tip of the turning tools being used for this.
- The following requirements apply if you want to use M128 for simultaneous turning:
- Only for NC programs programmed on the path of the tool center.
- Only for button turning tools with TO 9
- The tool must be measured at the center of the tool-tip radius
Subgroups of technology-specific tool types
Example
- An NC program with simultaneous turning includes the following components:
- Activate turning mode
- Insert a turning tool
- Adjust the coordinate system with cycle 800 ADJUST XZ SYSTEM
- Activate FUNCTION TCPM with REFPNT TIP-CENTER
- Activate cutter radius compensation with RL/RR
- Program simultaneous turning contour
- End cutter radius compensation with R0 or by departing the contour
- Reset FUNCTION TCPM
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.
0 BEGIN PGM TURNSIMULTAN MM | |||
* - ... | |||
12 FUNCTION MODE TURN | ; Activate turning mode | ||
13 TOOL CALL "TURN_FINISH" | ; Insert turning tool | ||
14 FUNCTION TURNDATA SPIN VCONST:OFF S500 | |||
15 M140 MB MAX | |||
* - ... | ; Adjust the coordinate system | ||
16 CYCL DEF 800 ADJUST XZ SYSTEM ~ | |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
17 FUNCTION TCPM F TCP AXIS POS PATHCTRL AXIS REFPNT TIP-CENTER | ; Activate FUNCTION TCPM | ||
18 FUNCTION TURNDATA CORR-TCS:Z/X DRS:-0.1 | |||
19 L X+100 Y+0 Z+10 R0 FMAX M304 | |||
20 L X+45 RR FMAX | ; Activate cutter radius compensation with RR | ||
* - ... | |||
26 L Z-12.5 A-75 | ; Program simultaneous turning contour | ||
27 L Z-15 | |||
28 CC X+69 Z-20 | |||
29 CP PA-90 A-45 DR- | |||
30 CP PA-180 A+0 DR- | |||
* - ... | |||
47 L X+100 Z-45 R0 FMAX | ; End cutter radius compensation with R0 | ||
48 FUNCTION RESET TCPM | ; Reset FUNCTION TCPM | ||
49 FUNCTION MODE MILL | |||
* - ... | |||
71 END PGM TURNSIMULTAN MM |