Cycle 200 DRILLING
ISO programming
G200
Application
Related topics
- Cycle 203 UNIVERSAL DRILLING optionally with decreasing infeed, dwell time and chip breaking
- Cycle 205 UNIVERSAL PECKING optionally with with decreasing infeed, chip breaking, recessed starting point and advanced stop distance
- Cycle 241 SINGLE-LIP D.H.DRLNG optionally with recessed starting point, dwell depth, direction of rotation and speed when entering and leaving the hole
Cycle run
- The control positions the tool in the spindle axis at rapid traverse FMAX to the entered set-up clearance above the workpiece surface
- The tool drills to the first plunging depth at the programmed feed rate F
- The control retracts the tool at FMAX to set-up clearance, dwells there (if a dwell time was entered), and then moves at FMAX to set-up clearance above the first plunging depth
- The tool then drills deeper by the plunging depth at the programmed feed rate F.
- The control repeats this procedure (steps 2 to 4) until the programmed depth is reached (the dwell time from Q211 is effective with every infeed)
- Finally, the tool path is retracted from the hole bottom at rapid traverse FMAX to setup clearance or to 2nd setup clearance. The 2nd set-up clearance Q204 will only come into effect if its value is greater than the set-up clearance Q200
Notes
- Enter depth as negative
- Use the machine parameter displayDepthErr (no. 201003) to specify whether the control should display an error message (on) or not (off) if a positive depth is entered
- This cycle monitors the defined usable length LU of the tool. If the LU value is less than the DEPTH Q201, the control will display an error message.
Notes on programming
- Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0.
- The algebraic sign for the DEPTH cycle parameter determines the working direction. If you program DEPTH=0, the cycle will not be executed.
- This cycle monitors the defined usable length LU of the tool. If the LU value is less than the DEPTH Q201, the control will display an error message.
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.
Cycle parameters
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. The depth does not have to be a multiple of the plunging depth. The control will go to depth in one movement if:
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? (optional) Time in seconds that the tool remains at the hole bottom. Input: 0...3600.0000 or PREDEF | |
Q395 Diameter as reference (0/1)? (optional) 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.
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 200 DRILLING ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 L X+30 Y+20 FMAX M3 | ||
13 CYCL CALL | ||
14 L X+80 Y+50 FMAX M99 |