Cycle 821 SHOULDER, FACE
ISO programming
G821
Application
Refer to your machine manual.
This function must be enabled and adapted by the machine manufacturer.
This cycle enables you to face turn right-angled shoulders.
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 tool is outside the contour to be machined when the cycle is called, the cycle runs outside machining. If the tool is inside the contour to be machined, the cycle runs inside machining.
Related topics
- Cycle 822 SHOULDER, FACE. EXT., optionally a chamfer or a rounding arc at the beginning or the end of a contour, angle for plane and circumferential surface and radius at the contour corner
Roughing cycle sequence
The cycle machines the area from the cycle starting point to the end point defined in the cycle.
- 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 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
- The control moves the tool in the Z coordinate to the set-up clearance Q460. The movement is performed at rapid traverse.
- The control performs a paraxial infeed movement at rapid traverse.
- The control finishes the contour of the finished part 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
- 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.
- 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.
Note on programming
- Program a positioning block to the starting position with radius compensation R0 before the cycle call.
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 | |
Q493 Diameter at end of contour? X coordinate of the contour end point (diameter value) Input: –99999.999...+99999.999 | |
Q494 Contour end in Z? Z coordinate of the contour end point Input: –99999.999...+99999.999 | |
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 | |
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 821 SHOULDER, FACE ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 L X+75 Y+0 Z+2 FMAX M303 | ||
13 CYCL CALL |