ISO programming
G292
G292
Refer to your machine manual.
This function must be enabled and adapted by the machine manufacturer.
Cycle 292 INTERPOLATION TURNING CONTOUR FINISHING couples the tool spindle to the positions of the linear axes. This cycle enables you to machine specific rotationally symmetrical contours in the active working plane. You can also run this cycle in the tilted working plane. The center of rotation is the starting point in the working plane at the time the cycle is called. After executing this cycle, the control deactivates the spindle coupling again.
Before using Cycle 292, you first need to define the desired contour in a subprogram and reference this contour with Cycle 14 or SEL CONTOUR. Program the contour either with monotonically decreasing or monotonically increasing coordinates. Undercuts cannot be machined with this cycle. If you enter Q560=1, you can turn the contour and the cutting edge is oriented toward the circle center. If you enter Q560=0, you can mill the contour and the spindle is not oriented toward the circle center.
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.
Outside machining Q529 = 1 | Inside machining Q529 = 0 |
The control will, under no circumstances, output M5 before.
Help graphic | Parameter |
---|---|
Q560 Spindle coupling (0=off, 1=on)? Define whether the spindle will be coupled or not. 0: Spindle coupling off (mill the contour) 1: Spindle coupling on (turn the contour) 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 | |
Q546 Reverse tool rotation direction? Direction of spindle rotation of the active tool: 3: Clockwise rotating tool (M3) 4: Counter-clockwise rotating tool (M4) Input: 3, 4 | |
Q529 Machining operation (0/1)? Define whether an inside or outside contour will be machined: +1: Inside machining 0: Outside machining Input: 0, 1 | |
Q221 Oversize for surface? Allowance in the working plane Input: 0...99.999 | |
Q441 Infeed per revolution [mm/rev]? Dimension by which the control moves the tool during one revolution. Input: 0,001...99.999 | |
Q449 Feed rate / cutting speed? (mm/min) Feed rate relative to the contour starting point Q491. The feed rate of the tool center point path is adjusted depending on the tool radius and Q529 MACHINING OPERATION. From these parameters, the control determines the programmed cutting speed at the diameter of the contour starting point. Q529 = 1: Feed rate of the tool center point path is reduced for inside machining. Q529 = 0: Feed rate of the tool center point path is increased for outside machining. Input: 1...99999 or FAUTO | |
Q491 Contour starting point (radius)? Radius of the contour starting point (e.g., X coordinate, if tool axis is Z). This value has an absolute effect. Input: 0.9999...99999.9999 | |
Q357 Safety clearance to the side? Set-up clearance to the side of the workpiece when the tool approaches the first plunging depth. This value has an incremental effect. Input: 0...99999.9999 | |
Q445 Clearance height? Absolute height at which collision between tool and workpiece is impossible. The tool retracts to this position at the end of the cycle. Input: –99999.9999...+99999.9999 | |
Q592 Type of dimension (0/1)? Interpretation of the contour dimensions: 0: The control interprets the contour in the ZX coordinate plane. The control interprets the X axis values as radii. The coordinate system is left-handed. Therefore, the programmed direction of rotation for circles is as follows:
1: The control interprets the contour in the ZXØ coordinate plane. The control interprets the X axis values as diameters. The coordinate system is right-handed. Therefore, the programmed direction of rotation for circles is as follows:
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 292 CONTOUR.TURNG.INTRP. ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|
Before using Cycle 292, you first need to define the desired turning contour in a subprogram and refer to this contour with Cycle 14 or SEL CONTOUR. Describe the turning contour on the cross section of a rotationally symmetrical body. Depending on the tool axis, use the following coordinates to define the turning contour:
Tool axis used | Axial coordinate | Radial coordinate |
---|---|---|
Z | Z | X |
X | X | Y |
Y | Y | Z |
Example: If you are using the tool axis Z, program the turning contour in the axial direction in Z and the radius or diameter of the contour in X.
You can use this cycle for inside and outside machining. Some of the notes given in chapter Notes are illustrated in the following. You will also find an example in Example: Interpolation Turning Cycle 292
Inside machining
Outside machining
Overview
Depending on the entry for parameter Q560 you can either mill (Q560=0) or turn (Q560=1) the contour. For each of the two machining modes, there are different possibilities to define the tool in the tool table. This section describes the different possibilities:
Spindle coupling off, Q560=0
Milling: Define the milling cutter in the tool table as usual by entering the length, radius, toroid cutter radius, etc.
Spindle coupling on, Q560=1
Turning: The geometry data of the turning tool are converted to the data of a milling cutter. You now have the following three 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). 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) and parameter Q336.
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 | 8,9 | ORI + Q336 |
Interpolation turning, inside | 8,9 | ORI + Q336 |