ISO programming
G800
G800
Refer to your machine manual.
This function must be enabled and adapted by the machine manufacturer.
The cycle is machine-dependent.
To be able to perform a turning operation, you need to position the tool appropriately relative to the turning spindle. For this purpose, you can use Cycle 800 ADJUST XZ SYSTEM.
With turning operations, the inclination angle between the tool and turning spindle is important, for example to machine contours with undercuts. Cycle 800 provides various possibilities for aligning the coordinate system for an inclined machining operation:
If the milling spindle axis and the turning spindle axis are parallel to each other, you can use the Precession angle Q497 to define any desired rotation of the coordinate system about the spindle axis (Z axis). This may be necessary if you have to bring the tool into a specific position due to space restrictions or if you want to improve your ability to observe a machining process. If the turning spindle and milling spindle axes are not parallel, only two precession angles are realistic for machining. The control selects the angle that is closest to the input value of Q497.
Cycle 800 positions the milling spindle such that the cutting edge is aligned relative to the turning contour. You can use a mirrored version of the tool (REVERSE TOOL Q498); this offsets the milling spindle by 180°. In this way, you can use your tools for both inside and outside machining. Position the cutting edge at the center of the turning spindle by using a positioning block, such as L Y+0 R0 FMAX.
Sometimes it is not possible to clamp a workpiece such that the axis of rotation is aligned with the axis of the turning spindle. For example, this is the case with large or rotationally non-symmetric workpieces. The eccentric turning Q535 function in Cycle 800 enables you to perform turning in such cases as well.
During eccentric turning, more than one linear axis is coupled to the turning spindle. The control compensates the eccentricity by performing circular compensating movements with the coupled linear axes.
This function must be enabled and adapted by the machine manufacturer.
If you machine with high speed and a high amount of eccentricity, you need to program large feed rates for the linear axes in order to perform the movements synchronously. If these feed rates are not met, the contour would be damaged. The control therefore generates an error message if 80 % of a maximum axis speed or acceleration is exceeded. If this occurs, reduce the speed.
With Cycle 800 ADJUST XZ SYSTEM, the control aligns the workpiece coordinate system and orients the tool correspondingly. Cycle 800 is effective until it is reset by Cycle 801, or until Cycle 800 is redefined. Some cycle functions of Cycle 800 are implicitly reset by other factors:
The machine manufacturer configures your machine tool. If the tool spindle was defined as an axis in the kinematic model during this configuration, the feed-rate potentiometer is effective for movements related to Cycle 800.
The machine manufacturer can configure a grid for the positioning of the tool spindle.
Taking rotary axes into account during machining operations with M138
Help graphic | Parameters |
---|---|
Q497 Precession angle? Angle at which the control positions the tool. Input: 0.0000...359.9999 | |
Q498 Reverse tool (0=no/1=yes)? Mirror tool for inside/outside machining. Input: 0, 1 | |
Q530 Inclined machining? Position the tilting axes for inclined machining: 0: Maintain tilting axis position (axis must be positioned beforehand) 1: Automatically position the tilting axis, and orient the tool tip (MOVE). The relative position between the workpiece and tool remains unchanged. The control performs a compensating movement with the linear axes 2: Automatically position the tilting axis without orienting the tool tip (TURN) 3: Do not position the tilting axis. Position the tilting axes later in a separate positioning block (STAY). The control stores the position values in the parameters Q120 (A axis), Q121 (B axis) and Q122 (C axis). Input: 0, 1, 2, 3 | |
Q531 Angle of incidence? Angle of incidence for positioning the tool Input: -180...+180 | |
Q532 Feed rate for positioning? Traversing speed of the tilting axis during automatic positioning Input: 0.001...99999.999, or FMAX | |
Q533 Preferred dir. of incid. angle? 0: Solution that is the shortest distance from the current position -1: Solution that is in the range between 0° and -179.9999° +1: Solution that is in the range between 0° and +180° -2: Solution that is in the range between -90° and -179.9999° +2: Solution that is between +90° and +180° Input: –2, –1, 0, +1, +2 | |
Q535 Eccentric turning? Couple the axes for the eccentric turning operation: 0: Deactivate axis couplings 1: Activate axis couplings. The center of rotation is located at the active preset 2: Activate axis couplings. The center of rotation is located at the active datum 3: Do not change the axis couplings Input: 0, 1, 2, 3 | |
Q536 Eccentric turning without stop? Interrupt program run before the axes are coupled: 0: Stop before the axes are coupled again. In stopped condition, the control opens a window in which the amount of eccentricity and the maximum deflection of the individual axes are displayed. You can then continue the machining operating with NC-Start or select ABBRUCH 1: Axes are coupled without stopping beforehand Input: 0, 1 | |
Q599 or QS599 Retraction path/macro? Retraction prior to execution of positioning movements in the rotary axis or tool axis: 0: No retraction –1: Maximum retraction with M140 MB MAX, see Retracting in the tool axis with M140 > 0: Path for the retraction in mm or inches "...": Path for an NC program that will be called as a user macro. Input: –1...9999 in the case of text entry: maximum 255 characters or QS parameter |
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.
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 CYCL DEF 800 ADJUST XZ SYSTEM ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|
The user macro is another NC program.
A user macro contains a sequence of multiple instructions. With a macro, you can define multiple NC functions that the control executes. As a user, you create macros as an NC program.
Macros work in the same manner as NC programs that are called with the PGM CALL function, for example. You define a macro as an NC program with the file type *.h or *.i.
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.
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 RET MM | |
1 FUNCTION RESET TCPM | ; Reset TCPM |
2 L Z-1 R0 FMAX M91 | ; Traverse with M91 |
3 FN 10: IF +Q533 NE +0 GOTO LBL "DEF_DIRECTION" | ; If Q533 (preferred direction from Cycle 800) is not equal to 0, then jump to LBL "DEF_DIRECTION" |
4 FN 18: SYSREAD QL1 = ID240 NR1 IDX4 | ; Read system data (nominal position in the REF system) and store in QL1 |
5 QL0 = 500 * SGN QL1 | ; SGN = Check algebraic sign |
6 FN 9: IF +0 EQU +0 GOTO LBL "MOVE" | ; Jump to LBL MOVE |
7 LBL "DIRECTION" | |
8 QL0 = 500 * SGN Q533 | ; SGN = Check algebraic sign |
9 LBL "MOVE" | |
10 L X-500 Y+QL0 R0 FMAX M91 | ; Retraction with M91 |
11 END PGM RET MM |