ISO programming
G125
G125
In conjunction with Cycle 14 CONTOUR, this cycle enables you to machine open and closed contours.
Cycle 25 CONTOUR TRAIN offers considerable advantages over machining a contour using positioning blocks:
Help graphic | Parameter |
---|---|
Q1 Milling depth? Distance between workpiece surface and contour floor. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
Q3 Finishing allowance for side? Finishing allowance in the working plane. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
Q5 Workpiece surface coordinate? Absolute coordinate of the top surface of the workpiece Input: –99999.9999...+99999.9999 | |
Q7 Clearance height? Height at which the tool cannot collide with the workpiece (for intermediate positioning and retraction at the end of the cycle). This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q10 Plunging depth? Tool infeed per cut. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
Q11 Feed rate for plunging? Traversing feed rate in the spindle axis Input: 0...99999.9999 or FAUTO, FU, FZ | |
Q12 Feed rate for roughing? Traversing feed rate in the working plane Input: 0...99999.9999 or FAUTO, FU, FZ | |
Q15 Climb or up-cut? up-cut = -1 +1: Climb milling –1: Up-cut milling 0: Climb milling and up-cut milling alternately in several infeeds Input: -1, 0, +1 | |
Q18 or QS18 Coarse roughing tool? Number or name of the tool with which the control has already coarse-roughed the contour. You are able to transfer the coarse roughing tool directly from the tool table via the action bar. In addition, you can enter the tool name via Name in the action bar. The control automatically inserts the closing quotation mark when you exit the input field. If there was no coarse roughing, enter "0"; if you enter a number or a name, the control will only rough-out the portion that could not be machined with the coarse roughing tool. If the portion to be roughed cannot be approached from the side, the control will mill in a reciprocating plunge-cut; for this purpose you must enter the tool length LCUTS in the TOOL.T tool table and define the maximum plunging angle of the tool with ANGLE. Input: 0...99999.9 or max. 255 characters | |
Q446 Accepted residual material? Specify the maximum value in mm up to which you accept residual material on the contour. For example, if you enter 0.01 mm, the control will stop machining residual material when it has reached a thickness of 0.01 mm. Input: 0.001...9.999 | |
Q447 Maximum connection distance? Maximum distance between two areas to be fine-roughed. Within this distance, the tool will move along the contour without lift-off movement, remaining at machining depth. Input: 0...999.999 | |
Q448 Path extension? Length by which the tool path is extended at the beginning and end of a contour area. The control always extends the tool path in parallel to the contour. Input: 0...99.999 |
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 25 CONTOUR TRAIN ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|