ISO programming
G122
G122
Use Cycle 22 ROUGH-OUT to define the technology data for roughing.
This cycle might require a center-cut end mill (ISO 1641) or pilot drilling with Cycle 21.
Help graphic | Parameter |
---|---|
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 | |
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 | |
Q19 Feed rate for reciprocation? Reciprocation feed rate in mm/min Input: 0...99999.9999 or FAUTO, FU, FZ | |
Q208 Feed rate for retraction? Tool traversing speed in mm/min when retracting after the machining operation. If you enter Q208 = 0, the control retracts the tool at the feed rate specified in Q12. Input: 0...99999.9999 or FMAX, FAUTO, PREDEF | |
Q401 Feed rate factor in %? Percentage value to which the control reduces the machining feed rate (Q12) as soon as the tool moves with its entire circumference within the material during roughing. If you use the feed rate reduction, then you can define the feed rate for roughing so large that there are optimum cutting conditions with the path overlap (Q2) specified in Cycle 20. The control then reduces the feed rate as per your definition at transitions and narrow places, reducing the total machining time. Input: 0.0001...100 | |
Q404 Fine roughing strategy (0/1)? Define how the control will move the tool during fine roughing when the radius of the fine-roughing tool is equal to or larger than half the radius of the coarse roughing tool. 0: Between areas that need to be fine-roughed, the control moves the tool along the contour at the current depth 1: Between areas that need to be fine-roughed, the control retracts the tool to set-up clearance and then moves it to the starting point of the next area to be roughed out Input: 0, 1 |
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 22 ROUGH-OUT ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|