ISO programming
G233
G233
With Cycle 233, you can face-mill a level surface in multiple infeeds while taking the finishing allowance into account. You can also define side walls in the cycle, which are then taken into account when machining the level surface. The cycle offers you various machining strategies:
![]() | ![]() |
The strategies Q389=0 and Q389=1 differ in the overtravel during face milling. If Q389=0, the end point lies outside of the surface, with Q389=1, it lies at the edge of the surface. The control calculates end point 2 from the side length and the set-up clearance to the side. If the strategy Q389=0 is used, the control additionally moves the tool beyond the level surface by the tool radius.
![]() | ![]() |
The strategies Q389=2 and Q389=3 differ in the overtravel during face milling. If Q389=2, the end point lies outside of the surface, with Q389=3, it lies at the edge of the surface. The control calculates end point 2 from the side length and the set-up clearance to the side. If the strategy Q389=2 is used, the control additionally moves the tool beyond the level surface by the tool radius.
If you program a lateral limitation, the control might not be able to perform movements outside of the contour. In this case the cycle runs as follows:
The limits enable you to set limits to the machining of the level surface so that, for example, side walls or shoulders are considered during machining. A side wall that is defined by a limit is machined to the finished dimension resulting from the starting point or the side lengths of the level surface. During roughing the control takes the allowance for the side into account, whereas during finishing the allowance is used for pre-positioning the tool.
Enter Q204 2ND SET-UP CLEARANCE in such a way that no collision with the workpiece or the fixtures can occur.
Help graphic | Parameter |
---|---|
Q215 Machining operation (0/1/2)? Define the machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing Input: 0, 1, 2 | |
Q389 Machining strategy (0-4)? Specify how the control machines the surface: 0: Meander machining, stepover at positioning feed rate outside the surface to be machined 1: Meander machining, stepover at the feed rate for milling at the edge of the surface to be machined 2: Machining line by line, retraction and stepover at positioning feed rate outside the surface to be machined 3: Machining line by line, retraction and stepover at positioning feed rate at the edge of the surface to be machined 4: Helical machining, uniform infeed from the outside toward the inside Input: 0, 1, 2, 3, 4 | |
Q350 Milling direction? Axis in the working plane that defines the machining direction: 1: Main axis = Machining direction 2: Secondary axis = Machining direction Input: 1, 2 | |
Q218 First side length? Length of the surface to be machined in the main axis of the working plane, referencing the starting point in the 1st axis. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
Q219 Second side length? Length of the surface to be machined in the secondary axis of the working plane. Use algebraic signs to specify the direction of the first cross feed referenced to the STARTNG PNT 2ND AXIS. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
Q227 Starting point in 3rd axis? Coordinate of the workpiece surface used to calculate the infeeds. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q386 End point in 3rd axis? Coordinate in the spindle axis on which the surface will be face-milled. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q369 Finishing allowance for floor? Value used for the last infeed. This value has an incremental effect. Input: 0...99999.9999 | |
Q202 Maximum plunging depth? Infeed per cut. Enter an incremental value greater than 0. Input: 0...99999.9999 | |
Q370 Path overlap factor? Maximum stepover factor k. The control calculates the actual stepover from the second side length (Q219) and the tool radius so that a constant stepover is used for machining. Input: 0.0001...1.9999 | |
Q207 Feed rate for milling? Traversing speed of the tool in mm/min for milling Input: 0...99999.999 or FAUTO, FU, FZ | |
Q385 Finishing feed rate? Traversing speed of the tool in mm/min while milling the last infeed Input: 0...99999.999 or FAUTO, FU, FZ | |
Q253 Feed rate for pre-positioning? Traversing speed of the tool in mm/min when approaching the starting position and when moving to the next pass. If you are moving the tool transversely inside the material (Q389=1), the control uses the cross feed rate for milling Q207. Input: 0...99999.9999 or FMAX, FAUTO, PREDEF | |
Q357 Safety clearance to the side? Parameter Q357 influences the following situations: Approaching the first infeed depth: Q357 is the lateral distance from the tool to the workpiece. Roughing with the Q389 = 0 to 3 roughing strategies: The surface to be machined is extended in Q350 MILLING DIRECTION by the value from Q357 if no limit has been set in that direction. Side finishing: The paths are extended by Q357 in the Q350 MILLING DIRECTION. This value has an incremental effect. Input: 0...99999.9999 | |
Q200 Set-up clearance? Distance between tool tip and workpiece surface. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
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 | |
Q347 1st limit? Select the side of the workpiece where the plane surface is bordered by a side wall (not possible with helical machining). Depending on the position of the side wall, the control limits the machining of the plane surface to the corresponding starting point coordinate or side length: 0: No limitation -1: Limit in negative main axis +1: Limit in positive main axis -2: Limit in negative secondary axis +2: Limit in positive secondary axis Input: –2, –1, 0, +1, +2 | |
Q348 2nd limit? See parameter Q347 1st limit Input: –2, –1, 0, +1, +2 | |
Q349 3rd limit? See parameter Q347 1st limit Input: –2, –1, 0, +1, +2 | |
Q368 Finishing allowance for side? Finishing allowance in the working plane. 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 | |
Q367 Surface position (-1/0/1/2/3/4)? Position of the surface relative to the position of the tool when the cycle is called: -1: Tool position = Current position 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: –1, 0, +1, +2, +3, +4 |
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 233 FACE MILLING ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 L X+50 Y+50 R0 FMAX M99 |