Cycle 201 REAMING
ISO programming
G201
Application
Cycle sequence
- 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 reams to the entered depth at the programmed feed rate F.
- If programmed, the tool remains at the hole bottom for the entered dwell time.
- Then, the control retracts the tool 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.
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 reaming Input: 0...99999.999 or FAUTO, FU | |
Q211 Dwell time at the depth? Time in seconds that the tool remains at the hole bottom. Input: 0...3600.0000 or PREDEF | |
Q208 Feed rate for retraction? Traversing speed of the tool in mm/min when retracting from the hole. If you enter Q208 = 0, the feed rate for reaming applies. Input: 0...99999.9999 or FMAX, FAUTO, 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 |
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 201 REAMING ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 L X+30 Y+20 FMAX M3 | ||
13 CYCL CALL |