Cycle 25 CONTOUR TRAIN
ISO programming
G125
Application
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:
- The control monitors the operation to prevent undercuts and contour damage (run a graphic simulation of the contour before execution)
- If the radius of the selected tool is too large, the corners of the contour may have to be reworked
- Machining can be done throughout by up-cut or by climb milling. The type of milling will even be retained if the contours were mirrored
- The tool can traverse back and forth for milling in several infeeds: This results in faster machining
- Allowance values can be entered in order to perform repeated rough-milling and finish-milling operations.
Notes
- After the end of the cycle, position the tool with all coordinates of the working plane (e.g., L X+80 Y+0 R0 FMAX)
- Make sure to program an absolute position after the cycle; do not program an incremental traversing movement
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- The control takes only the first label of Cycle 14 CONTOUR into account.
- The memory capacity for programming an SL cycle is limited. You can program up to 16384 contour elements in one SL cycle.
- If M110 is activated during operation, the feed rate for arcs compensated on the inside will be reduced accordingly.
- The cycle considers the miscellaneous functions M109 and M110. During the inside and outside machining of circular arcs the control keeps the feed rate constant at the cutting edge for inside and outside radii.
Notes on programming
- Cycle 20 CONTOUR DATA, is not required.
- The algebraic sign for the DEPTH cycle parameter determines the working direction. If you program DEPTH=0, the cycle will not be executed.
- If you use local QL Q parameters in a contour subprogram, you must also assign or calculate these in the contour subprogram.
Cycle parameters
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? (optional) Number or name of the tool with which the control has already coarse-roughed the contour. You can use the action bar selection to apply the coarse roughing tool directly from the tool table. In addition, you can enter the tool name yourself by selecting 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? (optional) 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? (optional) 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? (optional) 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.
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 25 CONTOUR TRAIN ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|