ISO programming
G813
G813
Refer to your machine manual.
This function must be enabled and adapted by the machine manufacturer.
This cycle enables you to run longitudinal turning of shoulders with plunging elements (undercuts).
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.
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 Q492 Contour start in Z, the control positions the tool in the Z coordinate to set-up clearance and begins the cycle there.
In undercutting, the control uses feed rate Q478 for the infeed. The control always retracts the tool to the set-up clearance.
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 contour starting point (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 the line perpendicular to the rotary axis. Input: 0...89.9999 | |
Q463 Maximum cutting depth? Maximum infeed (radius value) in the radial 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 813 TURN PLUNGE CONTOUR LONGITUDINAL ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 L X+75 Y+0 Z+2 R0 FMAX M303 | ||
13 CYCL CALL |