ISO programming
G200
G200
With this cycle, you can drill basic holes. In this cycle, the depth reference is selectable.
If you want to drill without chip breaking, make sure to define, in the Q202 parameter, a higher value than the depth Q201 plus the calculated depth based on the point angle. You can enter a much higher value there.
Help graphic | Parameter |
---|---|
Q200 Set-up clearance? Distance between tool tip 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 while drilling Input: 0...99999.999 or FAUTO, FU | |
Q202 Plunging depth? Tool infeed per cut. This value has an incremental effect.
Input: 0...99999.9999 | |
Q210 Dwell time at the top? Time in seconds that the tool remains at set-up clearance after having been retracted from the hole for chip removal. Input: 0...3600.0000 or PREDEF | |
Q203 Workpiece surface coordinate? Coordinate on the workpiece surface referenced to the active preset. 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 | |
Q211 Dwell time at the depth? Time in seconds that the tool remains at the hole bottom. Input: 0...3600.0000 or PREDEF | |
Q395 Diameter as reference (0/1)? Select whether the entered depth is referenced to the tool tip or the cylindrical part of the tool. If the control is to reference the depth to the cylindrical part of the tool, the point angle of the tool must be defined in the T-ANGLE column of the tool table TOOL.T. 0 = Depth referenced to tool tip 1 = Depth referenced to the cylindrical part of the tool 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 200 DRILLING ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 L X+30 Y+20 FMAX M3 | ||
13 CYCL CALL | ||
14 L X+80 Y+50 FMAX M99 |