ISO programming
G208
G208
With this cycle, you can mill holes. In this cycle, you can define an optional, pre-drilled diameter. You can also program tolerances for the nominal diameter.
If you program Q370=0 for the path overlap, the control uses the greatest path overlap possible for the first helical path. The control does this to prevent the tool from contacting the workpiece surface. All other paths are distributed uniformly.
The control allows you to store tolerances in the parameter Q335 NOMINAL DIAMETER.
You can define the following tolerances:
Tolerance | Example | Manufacturing dimension |
---|---|---|
Deviations | 10+0.01-0.015 | 9.9975 |
DIN EN ISO 286-2 | 10H7 | 10.0075 |
ISO 2768-1 | 10m | 10.0000 |
Help graphic | Parameter |
---|---|
Q200 Set-up clearance? Distance between lower edge of tool and workpiece surface. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
Q201 Depth? Distance between workpiece surface and bottom of hole. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
Q206 Feed rate for plunging? Traversing speed of the tool in mm/min during helical drilling Input: 0...99999.999 or FAUTO, FU, FZ | |
Q334 Feed per revolution of helix Depth of the tool plunge with each helix (=360°). This value has an incremental effect. Input: 0...99999.9999 | |
Q203 Workpiece surface coordinate? Coordinate on the workpiece surface referenced to the active datum. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q204 2nd set-up clearance? Distance in the tool axis between tool and workpiece (fixtures) at which no collision can occur. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
Q335 Nominal diameter? Hole diameter. If you entered the nominal diameter to be the same as the tool diameter, the control will bore directly to the entered depth without any helical interpolation. This value has an absolute effect. You can program a tolerance if needed. Input: 0...99999.9999 | |
Q342 Roughing diameter? Enter the dimension of the pre-drilled diameter. This value has an absolute effect. Input: 0...99999.9999 | |
Q351 Direction? Climb=+1, Up-cut=-1 Type of milling operation. The direction of spindle rotation is taken into account. +1 = climb milling –1 = up-cut milling (if you enter 0, climb milling is performed) Input: -1, 0, +1 or PREDEF | |
Q370 Path overlap factor? The control uses the path overlap factor to determine the stepover factor k. 0: The control uses the greatest path overlap possible for the first helical path. The control does this to prevent the tool from contacting the workpiece surface. All other paths are distributed uniformly. >0: The control multiplies the factor by the active tool radius. The result is the stepover factor k. Input: 0.1...1999 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 208 BORE MILLING ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 CYCL CALL |