Cycle 292 CONTOUR.TURNG.INTRP. (#96 / #7-04-1)
ISO programming
G292
Application
Refer to your machine manual.
This function must be enabled and adapted by the machine manufacturer.
Cycle 292 CONTOUR.TURNG.INTRP. 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.
Cycle sequence
Cycle Q560=0: Contour milling
- The M3/M4 function programmed before the cycle call remains in effect.
- No spindle stop and no spindle orientation will be performed. Q336 is not taken into account
- The control positions the tool at the contour start radius Q491, taking the selected machining type (inside/outside, Q529) and the set-up clearance to the side (Q357) into account. The described contour is not automatically extended by a set-up clearance. An extension of the contour must be programmed in the subprogram.
- The control machines the defined contour using a rotating spindle (M3/M4). The principal axes of the working plane move on a circle, whereas the spindle axis does not follow.
- At the end point of the contour, the control retracts the tool perpendicularly to the set-up clearance.
- Finally, the control retracts the tool to the clearance height.
Cycle Q560=1: Contour turning
- The control orients the tool spindle to the specified center of rotation. The specified angle Q336 is taken into account. If an "ORI" value has been defined in the turning-tool table (toolturn.trn), it is also taken into account.
- The tool spindle is now coupled to the position of the linear axes. The spindle follows the nominal position of the reference axes.
- The control positions the tool at the contour start radius Q491, taking the selected machining operation (inside/outside, Q529) and the set-up clearance to the side, Q357, into account. The described contour is not automatically extended by a set-up clearance. An extension of the contour must be programmed in the subprogram.
- The control uses the interpolation turning cycle to machine the defined contour. In interpolation turning, the linear axes of the working plane move on a circle, whereas the spindle axis follows; it is oriented perpendicularly to the surface.
- At the end point of the contour, the control retracts the tool perpendicularly to the set-up clearance.
- Finally, the control retracts the tool to the clearance height.
- The control automatically undoes the coupling of the tool spindle to the linear axes.
Notes
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.
- Program an extension of the contour in the subprogram
- Make sure that there is no material at the contour starting point
- The center of the turning contour is the starting point in the working plane at the time the cycle is called
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- The cycle is CALL-active.
- Roughing operations with multiple passes are not possible in this cycle.
- For inside contours, the control checks whether the active tool radius is less than half the diameter at the start of contour Q491 plus the set-up clearance to the side Q357. If the control determines that the tool is too large, the NC program will be canceled.
- Remember that the axis angle must be equal to the tilt angle before the cycle call! Only then can the axis be correctly coupled.
- If Cycle 8 MIRRORING is active, the control does not execute the interpolation turning cycle.
- If Cycle 26 AXIS-SPECIFIC SCALING is active, and the scaling factor for the axis does not equal 1, the control does not perform the cycle for interpolation turning.
- Parameter Q449 FEED RATE is used to program the feed rate at the starting radius. Keep in mind that the feed rate in the status display is referenced to the TCP and may deviate from Q449. The control calculates the feed rate in the status display as follows.
Outside machining Q529 = 1
Inside machining Q529 = 0
Notes on programming
- Program the turning contour without tool radius compensation (RR/RL) and without APPR or DEP movements.
- Please note that it is not possible to define programmed finishing allowances via the FUNCTION TURNDATA CORR-TCS(WPL) function. Program a finishing allowance for your contour directly in the cycle or by specifying a tool compensation (DXL, DZL, DRS) in the tool table.
- When programming, remember to use only positive radius values.
- When programming, remember that neither the spindle center nor the indexable insert must be moved into the center of the turning contour.
- Program outside contours with a radius greater than 0.
- Program inside contours with a radius greater than the tool radius.
- In order to attain high contouring speeds for your machine, define a large tolerance with Cycle 32 before calling the cycle. Program Cycle 32 with HSC filter=1.
- If you deactivate the spindle coupling (Q560 = 0), you can execute this cycle with polar kinematics. This requires that you clamp the workpiece at the center of the rotary table.
Note regarding machine parameters
- With Q560=1, the control does not check whether the cycle is run with a rotating or stationary spindle. (Independent of CfgGeoCycle - displaySpindleError (no. 201002))
- In the machine parameter mStrobeOrient (no. 201005), the machine manufacturer defines the M function for spindle orientation.
- If the value is > 0, the control executes this M number to perform the oriented spindle stop (PLC function defined by the machine manufacturer). The control waits until the oriented spindle stop has been completed.
- The control will, under no circumstances, output M5 before.
- If you enter –1, the control will perform the oriented spindle stop.
- If you enter 0, no action will be taken.
Cycle parameters
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.
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 CYCL DEF 292 CONTOUR.TURNG.INTRP. ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|
Machining variants
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 with Cycle 292
Inside machining
- The center of rotation is the position of the tool in the working plane when the cycle is called (1)
- Once the cycle has started, do not move the indexable insert or the spindle center into the center of rotation. Keep this in mind while describing the contour! (2)
- The described contour is not automatically extended by a set-up clearance. An extension of the contour must be programmed in the subprogram.
- At the beginning of the machining operation, the control positions the tool to the contour starting point at rapid traverse in the tool axis direction. Make sure that there is no material at the contour starting point.
You also need to take the following into account when programming the inside contour:
- -Program either monotonously increasing radial and axial coordinates (e.g., 1 to 5)
- -Or program monotonously decreasing radial and axial coordinates (e.g., 5 to 1)
- -Program inside contours with a radius greater than the tool radius.
Outside machining
- The center of rotation is the position of the tool in the working plane when the cycle is called (1)
- Once the cycle has started, do not move the indexable insert or the spindle center into the center of rotation. Keep this in mind while describing the contour! (2)
- The described contour is not automatically extended by a set-up clearance. An extension of the contour must be programmed in the subprogram.
- At the beginning of the machining operation, the control positions the tool to the contour starting point at rapid traverse in the tool axis direction. Make sure that there is no material at the contour starting point.
You also need to take the following into account when programming the outside contour:
- -Program either monotonously increasing radial coordinates and monotonously decreasing axial coordinates (e.g., 1 to 5)
- -Or program monotonously decreasing radial coordinates and monotonously increasing axial coordinates (e.g., 5 to 1)
- -Program outside contours with a radius greater than 0.
Defining the tool
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:
- Define a turning tool in the tool table (tool.t) as a milling tool
- Define a milling tool in the tool table (tool.t) as a milling tool (for subsequent use as a turning tool)
- Define a turning tool in the turning tool table (toolturn.trn)
These three possibilities of defining the tool are described in more detail below:
- Define a turning tool in the tool table (tool.t) as a milling tool
If you are working without the Turning software option (#50 / #4-03-1), 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.
- NoticeDanger of collision!Collision may occur between the tool holder and workpiece during inside machining. The tool holder is not monitored. If the tool holder results in a larger rotational diameter than the cutter does, there is a danger of collision.
- Select the tool holder to ensure that it does not result in a larger rotational diameter than the cutter does
- Define a milling tool in the tool table (tool.t) as a milling tool (for subsequent use as a turning tool)
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.
- Define a turning tool in the turning tool table (toolturn.trn)
If you are working with the Turning software option (#50 / #4-03-1), 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
You can use the following tool types for interpolation turning:
- TYPE: ROUGH, with the machining directions TO: 1 or 7
- TYPE: FINISH, with the machining directions TO: 1 or 7
- TYPE: BUTTON, with the machining directions TO: 1 or 7
The following tool types cannot be used for interpolation turning:
- TYPE: ROUGH, with the machining directions TO: 2 to 6
- TYPE: FINISH, with the machining directions TO: 2 to 6
- TYPE: BUTTON, with the machining directions TO: 2 to 6
- TYPE: RECESS
- TYPE: RECTURN
- TYPE: THREAD