ISO programming
G824
G824
Refer to your machine manual.
This function must be enabled and adapted by the machine manufacturer.
This cycle enables you to run face turning of plunging elements (undercuts). Extended scope of function:
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 start diameter Q491 is larger than the end diameter Q493, the cycle runs outside machining. If the start diameter Q491 is less than the end diameter Q493, the cycle runs inside machining.
In undercutting, the control uses feed rate Q478 for the infeed. The control always retracts the tool to the set-up clearance.
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 set-up clearance and begins the cycle there.
Fundamentals of turning cycles
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 | |
Q491 Diameter at contour start? X coordinate of the starting point for the plunging path (diameter value) Input: –99999.999...+99999.999 | |
Q492 Contour start in Z? Z coordinate of the starting point for the plunging path Input: –99999.999...+99999.999 | |
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 | |
Q495 Angle of side? Angle of plunging flank. The reference angle is a line parallel to the rotary axis. Input: 0...89.9999 | |
Q501 Starting element type (0/1/2)? Define the type of element at the beginning of the contour (circumferential surface): 0: No additional element 1: Element is a chamfer 2: Element is a radius Input: 0, 1, 2 | |
Q502 Size of starting element? Size of the starting element (chamfer section) Input: 0...999.999 | |
Q500 Radius of the contour corner? Radius of the inside corner of the contour. If no radius is specified, the radius will be that of the indexable insert. Input: 0...999.999 | |
Q496 Angle of circumferen. surface? Angle between the circumferential surface and rotary axis Input: 0...89.9999 | |
Q503 End element type (0/1/2)? Define the type of element at the contour end (plane surface): 0: No additional element 1: Element is a chamfer 2: Element is a radius Input: 0, 1, 2 | |
Q504 Size of end element? Size of the end element (chamfer section) Input: 0...999.999 | |
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? Freed 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.
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 824 TURN PLUNGE TRANSVERSE EXT. ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 L X+75 Y+0 Z+2 FMAX M303 | ||
13 CYCL CALL |