Cycle 256 RECTANGULAR STUD
ISO programming
G256
Application
Cycle sequence
- The tool moves from the cycle starting position (stud center) to the starting position for stud machining. Specify the starting position with parameter Q437. The default position (Q437=0) is 2 mm to the right of the stud blank
- If the tool is at the 2nd set-up clearance, it moves at rapid traverse FMAX to set-up clearance, and from there advances to the first plunging depth at the feed rate for plunging
- The tool then moves tangentially to the stud contour and machines one revolution
- If the finished dimension cannot be machined with one revolution, the control performs a stepover with the current factor, and machines another revolution. The control takes the dimensions of the workpiece blank, the finished dimension, and the permitted stepover into account. This process is repeated until the defined finished dimension has been reached. If, on the other hand, you did not set the starting point on a side, but rather on a corner (Q437 not equal to 0), the control mills on a spiral path from the starting point inward until the finished dimension has been reached.
- If further stepovers are required, the tool is retracted from the contour on a tangential path and returns to the starting point of stud machining
- The control then plunges the tool to the next plunging depth, and machines the stud at this depth
- This process is repeated until the programmed stud depth is reached
- At the end of the cycle, the control positions the tool in the tool axis at the clearance height defined in the cycle. This means that the end position differs from the starting position
Notes
- Enter depth as negative
- Use the machine parameter displayDepthErr (no. 201003) to specify whether the control should display an error message (on) or not (off) if a positive depth is entered
- Depending on the approach position Q439, leave enough room next to the stud for the approach movement
- Leave room next to the stud for the approach motion
- At least tool diameter + 2 mm
- At the end, the control returns the tool to set-up clearance, or to 2nd set-up clearance if one was programmed. The end position of the tool after the cycle differs from the starting position.
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- The control automatically pre-positions the tool in the tool axis. Make sure to program Q204 2ND SET-UP CLEARANCE correctly.
- This cycle finishes Q369 ALLOWANCE FOR FLOOR with only one infeed. Parameter Q338 INFEED FOR FINISHING has no effect on Q369. Q338 is effective in finishing of Q368 ALLOWANCE FOR SIDE.
- The control reduces the plunging depth to the LCUTS cutting edge length defined in the tool table if the cutting edge length is shorter than the Q202 plunging depth programmed in the cycle.
- This cycle monitors the defined usable length LU of the tool. If the LU value is less than the DEPTH Q201, the control will display an error message.
Notes on programming
- Pre-position the tool in the working plane to the starting position with radius compensation R0. Note parameter Q367 (position).
- The algebraic sign for the DEPTH cycle parameter determines the working direction. If you program DEPTH=0, the cycle will not be executed.
Cycle parameters
Help graphic | Parameter |
---|---|
Q218 First side length? Length of stud parallel to the main axis of the working plane This value has an incremental effect. 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. This value has an incremental effect. 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. This value has an incremental effect. Input: 0...99999.9999 | |
Q425 Workpiece blank side length 2? Length of stud blank parallel to the secondary axis of the working plane. This value has an incremental effect. 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 machining plane which remains after roughing. 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)? (optional) 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)? (optional) Define the machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing Input: 0, 1, 2 | |
Q369 Finishing allowance for floor? (optional) Finishing allowance in depth which remains after roughing. This value has an incremental effect. Input: 0...99999.9999 | |
Q338 Infeed for finishing? (optional) Infeed in the tool axis when finishing the lateral finishing allowance Q368. This value has an incremental effect. 0: Finishing in one infeed Input: 0...99999.9999 | |
Q385 Finishing feed rate? (optional) 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.
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 256 RECTANGULAR STUD ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 L X+50 Y+50 R0 FMAX M99 |