Cycle 820 TURN CONTOUR TRANSV.
ISO programming
G820
Application
Refer to your machine manual.
This function must be enabled and adapted by the machine manufacturer.
This cycle enables you to execute face turning of workpieces with any turning contours. The contour description is in a subprogram.
You can use the cycle either for roughing, finishing or complete machining. Turning is run paraxially with roughing.
The cycle can be used for inside and outside machining. If the coordinate of the contour starting point is larger than that of the contour end point, the cycle runs outside machining. If the coordinate of the contour starting point is less than that of the contour end point, the cycle runs inside machining.
Roughing cycle sequence
The control uses the tool position as cycle starting point when the cycle is called. If the Z coordinate of the starting point is less than the contour starting point, the control positions the tool in the Z coordinate to the contour starting point and begins the cycle there.
- The control performs a paraxial infeed movement at rapid traverse. The control calculates the infeed value based on Q463 Maximum cutting depth.
- The control machines the area between the starting position and the end point in transverse direction. The transverse cut is run paraxially at the defined feed rate Q478.
- The control retracts the tool at the defined feed rate by the infeed value.
- The control returns the tool at rapid traverse to the beginning of cut.
- The control repeats this procedure (steps 1 to 4) until the contour is completed.
- The control returns the tool at rapid traverse to the cycle starting point.
Finishing cycle sequence
If the Z coordinate of the starting point is less than the contour starting point, the control positions the tool in the Z coordinate to set-up clearance and begins the cycle there.
- The infeed movement is performed at rapid traverse.
- The control finishes the contour of the finished part (contour starting point to contour end point) at the defined feed rate Q505.
- The control retracts the tool at the defined feed rate to the set-up clearance.
- The control returns the tool at rapid traverse to the cycle starting point.
Notes
- Before calling the cycle, make sure to position the tool at the side of the cutting boundary (cutting limit) where the material will be machined
- This cycle can be executed only in the FUNCTION MODE TURN machining mode.
- The tool position at cycle call (cycle start point) influences the area to be machined.
- The control takes the cutting geometry of the tool into account to prevent damage to contour elements. If it is not possible to machine the entire workpiece with the active tool, the control will display a warning.
- If you programmed a value for CUTLENGTH, then it will be taken into account during the roughing operation in this cycle. A message is displayed and the plunging depth is automatically reduced.
- Also refer to the fundamentals of the turning cycles.
Notes on programming
- Program a positioning block to a safe position with radius compensation R0 before the cycle call.
- Before programming the cycle call, make sure to program Cycle 14 CONTOUR or SEL CONTOUR to be able to define the subprograms.
- If you use local QL Q parameters in a contour subprogram, you must also assign or calculate these in the contour subprogram.
- Finishing the contour requires programming tool radius compensation RL or RR in the contour description.
Cycle parameters
Help graphic | Parameter |
---|---|
Q215 Machining operation (0/1/2/3)? Define extent of machining: 0: Roughing and finishing 1: Only roughing 2: Only finishing to final dimension 3: Only finishing to oversize Input: 0, 1, 2, 3 | |
Q460 Set-up clearance? Distance for retraction and prepositioning. This value has an incremental effect. Input: 0...999.999 | |
Q499 Reverse the contour (0-2)? Define the machining direction of the contour: 0: Contour is executed in the programmed direction 1: Contour is executed in the direction opposite to the programmed direction 2: Contour is executed in the direction opposite to the programmed direction; the position of the tool is also adjusted Input: 0, 1, 2 | |
Q463 Maximum cutting depth? Maximum infeed in the axial direction. The infeed is distributed evenly to avoid abrasive cuts. Input: 0...99.999 | |
Q478 Roughing feed rate? Feed rate during roughing. If M136 has been programmed, the value is interpreted by the control in millimeters per revolution; without M136, in millimeters per minute. Input: 0...99999.999 or FAUTO | |
Q483 Oversize for diameter? Diameter oversize on the defined contour. This value has an incremental effect. Input: 0...99.999 | |
Q484 Oversize in Z? Oversize of the defined contour in the axial direction. This value has an incremental effect. Input: 0...99.999 | |
Q505 Finishing feed rate? Feed rate during finishing. If M136 has been programmed, the value is interpreted by the control in millimeters per revolution; without M136, in millimeters per minute. Input: 0...99999.999 or FAUTO | |
Q487 Allow plunging (0/1)? Permit the machining of plunging elements: 0: Do not machine any plunging elements 1: Machine plunging elements Input: 0, 1 | |
Q488 Feed rate for plunging (0=auto)? Definition of the feed rate during plunging. This input value is optional. If it is not programmed, then the feed rate defined for turning operations applies. Input: 0...99999.999 or FAUTO | |
Q479 Machining limits (0/1)? Activate cutting limit: 0: No cutting limit active 1: Cutting limit (Q480/Q482) Input: 0, 1 | |
Q480 Value of diameter limit? X value for contour limit (diameter value) Input: –99999.999...+99999.999 | |
Q482 Value of cutting limit in Z? Z value for contour limit Input: –99999.999...+99999.999 | |
Q506 Contour smoothing (0/1/2)? 0: Along the contour after every cut (within the infeed area) 1: Contour smoothing after the last cut (entire contour); retract by 45° 2: No contour smoothing; retract by 45° Input: 0, 1, 2 |
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 14.0 CONTOUR | ||
12 CYCL DEF 14.1 CONTOUR LABEL2 | ||
13 CYCL DEF 820 TURN CONTOUR TRANSV. ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
14 L X+75 Y+0 Z+2 FMAX M303 | ||
15 CYCL CALL | ||
16 M30 | ||
17 LBL 2 | ||
18 L X+75 Z-20 | ||
19 L X+50 | ||
20 RND R2 | ||
21 L X+20 Z-25 | ||
22 RND R2 | ||
23 L Z+0 | ||
24 LBL 0 |