Cycle 252 CIRCULAR POCKET
ISO programming
G252
Application
Cycle sequence
Roughing
- The control first moves the tool at rapid traverse to set-up clearance Q200 above the workpiece
- The tool plunges to the first plunging depth at the pocket center. Specify the plunging strategy with parameter Q366.
- The control roughs out the pocket from the inside out, taking the path overlap (Q370) and the finishing allowances (Q368 and Q369) into account.
- At the end of the roughing operation, the control moves the tool tangentially away from the pocket wall to set-up clearance Q200 in the working plane, then retracts the tool by Q200 at rapid traverse and returns it from there at rapid traverse to the pocket center
- Steps 2 to 4 are repeated until the programmed pocket depth is reached, taking the finishing allowance Q369 into account.
- If only roughing was programmed (Q215=1), the tool moves away from the pocket wall tangentially by the set-up clearance Q200, then retracts at rapid traverse to the second set-up clearance Q204 in the tool axis and returns at rapid traverse to the pocket center.
Finishing
- If finishing allowances have been defined, the control first finishes the pocket walls, in multiple infeeds, if so specified.
- The control positions the tool in the tool axis near the pocket wall at a distance corresponding to the finishing allowance Q368 plus the set-up clearance Q200
- The control roughs out the pocket from the inside out, until the diameter Q223 is reached
- Then, the control again positions the tool in the tool axis near the pocket wall at a distance corresponding to the finishing allowance Q368 plus the set-up clearance Q200 and repeats the finishing procedure for the side wall at the new depth
- The control repeats this process until the programmed diameter is reached
- After machining to the diameter Q223, the control retracts the tool tangentially by the finishing allowance Q368 plus the set-up clearance Q200 in the working plane, then retracts it at rapid traverse to set-up clearance Q200 in the tool axis and returns it to the pocket center.
- Next, the control moves the tool in the tool axis to the depth Q201 and finishes the floor of the pocket from the inside out. The tool approaches the pocket floor tangentially.
- The control repeats this process until the depth Q201 plus Q369 is reached.
- Finally, the tool moves away from the pocket wall tangentially by the set-up clearance Q200, then retracts at rapid traverse to set-up clearance Q200 in the tool axis and returns at rapid traverse to the pocket center.
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
- Conduct a roughing operation beforehand
- Ensure that the control can pre-position the tool at rapid traverse without colliding with the workpiece
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- The control automatically pre-positions the tool in the tool axis. Make sure to program Q204 2ND SET-UP CLEARANCE correctly.
- This cycle finishes Q369 ALLOWANCE FOR FLOOR with only one infeed. Parameter Q338 INFEED FOR FINISHING has no effect on Q369. Q338 is effective in finishing of Q368 ALLOWANCE FOR SIDE.
- The control reduces the plunging depth to the LCUTS cutting edge length defined in the tool table if the cutting edge length is shorter than the Q202 plunging depth programmed in the cycle.
- 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.
- Cycle 252 takes the cutting width RCUTS from the tool table.
Notes on programming
- If the tool table is inactive, you must always program vertical plunging (Q366=0) because a plunging angle cannot be defined.
- Pre-position the tool in the working plane to the starting position (circle center) 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.
- Program a sufficient set-up clearance so that the tool cannot jam because of chips.
Note regarding machine parameters
- For helical plunging, the control will display an error message if the internally calculated helix diameter is less than twice the tool diameter. If you are using a center-cut tool, you can switch this monitoring function off via the suppressPlungeErr machine parameter (no. 201006).
Cycle parameters
Help graphic | Parameter |
---|---|
Q215 Machining operation (0/1/2)? Define the machining operation: 0: Roughing and finishing 1: Only roughing 2: Only finishing Input: 0, 1, 2 | |
Q223 Circle diameter? Diameter of the finished pocket Input: 0...99999.9999 | |
Q368 Finishing allowance for side? Finishing allowance in the machining plane which remains after roughing. This value has an incremental effect. Input: 0...99999.9999 | |
Q207 Feed rate for milling? Traversing speed of the tool in mm/min for milling Input: 0...99999.999 or FAUTO, FU, FZ | |
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 PREDEF: The control uses the value of a GLOBAL DEF block (If you enter 0, climb milling is performed) Input: -1, 0, +1 or PREDEF | |
Q201 Depth? Distance between workpiece surface and bottom of pocket. This value has an incremental effect. Input: –99999.9999...+99999.9999 | |
Q202 Plunging depth? Tool infeed per cut. Enter a value greater than 0. This value has an incremental effect. Input: 0...99999.9999 | |
Q369 Finishing allowance for floor? Finishing allowance in depth which remains after roughing. This value has an incremental effect. Input: 0...99999.9999 | |
Q206 Feed rate for plunging? Traversing speed of the tool in mm/min for moving to depth Input: 0...99999.999 or FAUTO, FU, FZ | |
Q338 Infeed for finishing? Infeed in the tool axis when finishing the lateral finishing allowance Q368. This value has an incremental effect. 0: Finishing in one infeed Input: 0...99999.9999 | |
Q200 Set-up clearance? Distance between tool tip and workpiece surface. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
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? Coordinate in the spindle axis at which a collision between tool and workpiece (fixtures) is impossible. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
Q370 Path overlap factor? Q370x tool radius = stepover factor k. The overlap specified is the maximum overlap. The overlap can be reduced in order to prevent material from remaining at the corners. Input: 0.1...1999 or PREDEF | |
Q366 Plunging strategy (0/1)? Type of plunging strategy: 0: Vertical plunging. In the tool table, the plunging angle ANGLE for the active tool must be defined as 0 or 90. Otherwise, the control will display an error message 1: Helical plunging. In the tool table, the plunging angle ANGLE for the active tool must be defined as not equal to 0. Otherwise, the control will display an error message. If necessary, define the value of the RCUTS cutting width in the tool table Input: 0, 1 or PREDEF | |
Q385 Finishing feed rate? (optional) Traversing speed of the tool in mm/min for side and floor finishing Input: 0...99999.999 or FAUTO, FU, FZ | |
Q439 Feed rate reference (0-3)? (optional) Specify the reference for the programmed feed rate: 0: Feed rate is referenced to the path of the tool center 1: Feed rate is referenced to the cutting edge only during side finishing; otherwise, it is referenced to the path of the tool center 2: Feed rate is referenced to the cutting edge during side finishing and floor finishing; otherwise it is referenced to the path of the tool center 3: Feed rate is always referenced to the cutting edge Input: 0, 1, 2, 3 |
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 252 CIRCULAR POCKET ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 L X+50 Y+50 R0 FMAX M99 |
Plunging strategy Q366 with RCUTS
Behavior with RCUTS
Helical plunging Q366=1:
RCUTS > 0
- The control takes the cutting width RCUTS into account when calculating the helical path. The greater RCUTS, the smaller the helical path.
- Formula for calculating the helical radius:
Rcorr: Tool radius R + tool radius oversize DR
- If moving on a helical path is not possible due to limited space, the control will display an error message.
RCUTS = 0 or undefined
- suppressPlungeErr=on (no. 201006)
If moving on a helical path is not possible due to limited space, the control will reduce the helical path.
- suppressPlungeErr=off (no. 201006)
If moving on a helical radius is not possible due to limited space, the control will display an error message.