ISO programming
G232
G232
With Cycle 232, you can face-mill a level surface in multiple infeeds while taking the finishing allowance into account. Three machining strategies are available:
Enter Q204 2ND SET-UP CLEARANCE in such a way that no collision with the workpiece or the fixtures can occur.
Help graphic | Parameter |
---|---|
Q389 Machining strategy (0/1/2)? Define how the control will machine 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: Line-by-line machining, retraction and stepover at the positioning feed rate Input: 0, 1, 2 | |
Q225 Starting point in 1st axis? Define the starting point coordinate of the surface to be machined in the main axis of the working plane. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q226 Starting point in 2nd axis? Define the starting point coordinate of the surface to be machined in the secondary axis of the working plane. This value has an absolute 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 | |
Q218 First side length? Length of the surface to be machined in the main axis of the working plane. Use the algebraic sign to specify the direction of the first milling path referenced to 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 | |
Q202 Maximum plunging depth? Maximum infeed per cut. The control calculates the actual plunging depth from the difference between the end point and starting point in the tool axis (taking the finishing allowance into account), so that uniform plunging depths are used each time. This value has an incremental effect. Input: 0...99999.9999 | |
Q369 Finishing allowance for floor? Value used for the last infeed. This value has an incremental effect. Input: 0...99999.9999 | |
Q370 Max. 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. If you have entered a radius R2 in the tool table (e.g., cutter radius when using a face-milling cutter), the control reduces the stepover accordingly. Input: 0.001...1.999 | |
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 | |
Q200 Set-up clearance? Distance between tool tip and the starting position in the tool axis. If you are milling with machining strategy Q389 = 2, the control moves the tool to set-up clearance above the current plunging depth to the starting point of the next pass. This value has an incremental effect. Input: 0...99999.9999 or 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. Input: 0...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 |
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 232 FACE MILLING ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|