| 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? Reserved; currently no functionality |
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 |
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 |
| 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 |
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 |
| 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 |
Q507 Direction (0=bidir./1=unidir.)? Cutting direction: 0: Bidirectional (in both directions) 1: Unidirectional (in direction of contour) Input: 0, 1 |
Q508 Offset width? Reduction of the cutting length. After pre-cutting, the remaining material is removed with a single cut. If required, the control limits the programmed offset width. Input: 0...99.999 |
Q509 Depth compensat. for finishing? Depending on the material, feed rate, etc., the tool tip is displaced during an operation. You can correct the resulting infeed error with the depth compensation factor. Input: –9.9999...+9.9999 |
Q499 Reverse contour (0=no/1=yes)? Machining direction: 0: Machining in the direction of contour 1: Machining in the direction opposite to the contour direction Input: 0, 1 |