ISO programming
G291
G291
Refer to your machine manual.
This function must be enabled and adapted by the machine manufacturer.
Cycle 291 COUPLG.TURNG.INTERP. couples the tool spindle to the position of the linear axes, or cancels this spindle coupling. With interpolation turning, the cutting edge is oriented to the center of a circle. The center of rotation is defined in the cycle by entering the coordinates Q216 and Q217.
This cycle is effective only for machines with servo-controlled spindle.
Your control might monitor the tool to ensure that no positioning movements at feed rate are performed while spindle rotation is off. Contact the machine manufacturer for further information.
The control will, under no circumstances, output M5 before.
Help graphic | Parameter |
---|---|
Q560 Spindle coupling (0=off, 1=on)? Define whether the tool spindle will be coupled to the position of the linear axes. If spindle coupling is active, the tool's cutting edge is oriented to the center of rotation. 0: Spindle coupling off 1: Spindle coupling on Input: 0, 1 | |
Q336 Angle for spindle orientation? The control orients the tool to this angle before starting the machining operation. If you work with a milling tool, enter the angle in such a way that one cutting edge is turned towards the center of rotation. If you work with a turning tool, and have defined the value "ORI" in the turning tool table (toolturn.trn), then it is taken into account for the spindle orientation. Input: 0...360 | |
Q216 Center in 1st axis? Center of rotation in the main axis of the working plane Absolute input: –99999.9999...99999.9999 | |
Q217 Center in 2nd axis? Center of rotation in the secondary axis of the working plane Input: –99999.9999...+99999.9999 | |
Q561 Convert turning tool (0/1) Only relevant if you define the turning tool in the turning tool table (toolturn.trn). This parameter allows you to decide whether the value XL of the turning tool will be interpreted as radius R of a milling tool. 0: No change; the turning tool is interpreted as described in the turning tool table (toolturn.trn). In this case, you must not use the radius compensation RR or RL. Furthermore, you must describe the movement of the path of the tool center point TCP without spindle coupling when programming. This kind of programming is much more complicated. 1: The value XL from the turning tool table (toolturn.trn) is interpreted as a radius R of a milling tool table. This makes it possible to use radius compensation RR or RL when programming your contour. This kind of programming is recommended. Input: 0, 1 |
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 291 COUPLG.TURNG.INTERP. ~ | ||
| ||
| ||
| ||
| ||
|
Overview
Depending on the entry for parameter Q560 you can either activate (Q560=1) or deactivate (Q560=0) the COUPLG.TURNG.INTERP. cycle.
Spindle coupling off, Q560=0
The tool spindle is not coupled to the position of the linear axes.
Q560=0: Disable the COUPLG.TURNG.INTERP. cycle!
Spindle coupling on, Q560=1
A turning operation is executed with the tool spindle coupled to the position of the linear axes. If you set the parameter Q560=1, there are different possibilities to define the tool in the tool table. This section describes the different possibilities:
These three possibilities of defining the tool are described in more detail below:
If you are working without option 50, define your turning tool as a milling cutter in the tool table (tool.t). In this case, the following data from the tool table are taken into account (including delta values): length (L), radius (R), and corner radius (R2). The geometry data of the turning tool are converted to the data of a milling cutter. Align your turning tool to the spindle center. Specify this spindle orientation angle in parameter Q336 of the cycle. For outside machining, the spindle orientation equals the value in Q336, and for inside machining, the spindle orientation equals Q336+180.
You can perform interpolation turning with a milling tool. In this case, the following data from the tool table are taken into account (including delta values): length (L), radius (R), and corner radius (R2). Align one cutting edge of your milling cutter to the spindle center. Specify this angle in parameter Q336. For outside machining, the spindle orientation equals the value in Q336, and for inside machining, the spindle orientation equals Q336+180.
If you are working with option 50, you can define your turning tool in the turning tool table (toolturn.trn). In this case, the orientation of the spindle to the center of rotation takes place under consideration of tool-specific data, such as the type of machining (TO in the turning tool table), the orientation angle (ORI in the turning tool table), parameter Q336, and parameter Q561.
The spindle orientation is calculated as follows:
Machining | TO | Spindle orientation |
---|---|---|
Interpolation turning, outside | 1 | ORI + Q336 |
Interpolation turning, inside | 7 | ORI + Q336 + 180 |
Interpolation turning, outside | 7 | ORI + Q336 + 180 |
Interpolation turning, inside | 1 | ORI + Q336 |
Interpolation turning, outside | 8 | ORI + Q336 |
Interpolation turning, inside | 8 | ORI + Q336 |