ISO programming
G256
G256
Use Cycle 256 to machine a rectangular stud. If a dimension of the workpiece blank is greater than the maximum possible stepover, then the control performs multiple stepovers until the finished dimension has been machined.
Help graphic | Parameter |
---|---|
Q218 First side length? Length of stud parallel to the main axis of the working plane Input: 0...99999.9999 | |
Q424 Workpiece blank side length 1? Length of stud blank parallel to the main axis of the working plane. Enter Workpiece blank side length 1 greater than First side length. The control performs multiple lateral stepovers if the difference between blank dimension 1 and finished dimension 1 is greater than the permitted stepover (tool radius multiplied by path overlap Q370). The control always calculates a constant stepover. Input: 0...99999.9999 | |
Q219 Second side length? Length of stud parallel to the secondary axis of the working plane Enter Workpiece blank side length 2 greater than Second side length. The control performs multiple lateral stepovers if the difference between blank dimension 2 and finished dimension 2 is greater than the permitted stepover (tool radius multiplied by path overlap Q370). The control always calculates a constant stepover. Input: 0...99999.9999 | |
Q425 Workpiece blank side length 2? Length of stud blank parallel to the secondary axis of the working plane. Input: 0...99999.9999 | |
Q220 Radius / Chamfer (+/-)? Enter the value for the radius or chamfer form element. If you enter a positive value, the control will round every corner. The value you enter here refers to the radius. If you enter a negative value, all corners of the contour will be chamfered with the value entered as the length of the chamfer. Input: –99999.9999...+99999.9999 | |
Q368 Finishing allowance for side? Finishing allowance in the working plane, is left over after machining. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
Q224 Angle of rotation? Angle by which the entire operation is rotated. The center of rotation is the position at which the tool is located when the cycle is called. This value has an absolute effect. Input: –360.000...+360.000 | |
Q367 Position of stud (0/1/2/3/4)? Position of the stud with respect to the tool when the cycle is called. 0: Tool position = Center of stud 1: Tool position = Lower left corner 2: Tool position = Lower right corner 3: Tool position = Upper right corner 4: Tool position = Upper left corner Input: 0, 1, 2, 3, 4 | |
Q207 Feed rate for milling? Traversing speed of the tool in mm/min for milling Input: 0...99999.999 or FAUTO, FU, FZ | |
Q351 Direction? Climb=+1, Up-cut=-1 Type of milling operation. The direction of spindle rotation is taken into account. +1 = climb milling –1 = up-cut milling PREDEF: The control uses the value of a GLOBAL DEF block (If you enter 0, climb milling is performed) Input: -1, 0, +1 or PREDEF | |
Q201 Depth? Distance between workpiece surface and bottom of stud. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
Q202 Plunging depth? Tool infeed per cut. Enter a value greater than 0. This value has an incremental effect. Input: 0...99999.9999 | |
Q206 Feed rate for plunging? Traversing speed of the tool in mm/min while moving to depth Input: 0...99999.999 or FAUTO, FMAX, FU, FZ | |
Q200 Set-up clearance? Distance between tool tip and workpiece surface. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
Q203 Workpiece surface coordinate? Coordinate on the workpiece surface referenced to the active datum. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q204 2nd set-up clearance? Coordinate in the spindle axis at which a collision between tool and workpiece (fixtures) is impossible. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
Q370 Path overlap factor? Q370 x tool radius = stepover factor k. Input: 0.0001...1.9999 or PREDEF | |
Q437 Starting position (0...4)? Specify the approach strategy of the tool: 0: From the right of the stud (default setting) 1: Lower left corner 2: Lower right corner 3: Upper right corner 4: Upper left corner If approach marks appear on the stud surface during approach with the setting Q437=0, then choose another approach position. Input: 0, 1, 2, 3, 4 | |
Q215 Machining operation (0/1/2)? Define the machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing Input: 0, 1, 2 | |
Q369 Finishing allowance for floor? Finishing allowance for the floor. This value has an incremental effect. Input: 0...99999.9999 | |
Q338 Infeed for finishing? Tool infeed in the spindle axis per finishing cut. Q338 = 0: Finishing with a single infeed This value has an incremental effect. Input: 0...99999.9999 | |
Q385 Finishing feed rate? Traversing speed of the tool in mm/min for side and floor finishing Input: 0...99999.999 or FAUTO, FU, FZ |
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 256 RECTANGULAR STUD ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 L X+50 Y+50 R0 FMAX M99 |