Cycle 251 RECTANGULAR POCKET

ISO programming

G251

Application

Use Cycle 251 to completely machine rectangular pockets. Depending on the cycle parameters, the following machining alternatives are available:

  • Complete machining: Roughing, floor finishing, side finishing
  • Only roughing
  • Only floor finishing and side finishing
  • Only floor finishing
  • Only side finishing

Cycle sequence

Roughing

  1. The tool plunges into the workpiece at the pocket center and advances to the first plunging depth. Specify the plunging strategy with parameter Q366.
  2. The control roughs out the pocket from the inside out, taking the path overlap (Q370) and the finishing allowances (Q368 and Q369) into account.
  3. At the end of the roughing operation, the control moves the tool tangentially away from the pocket wall, then moves to set-up clearance above the current plunging depth. From there, the tool is returned at rapid traverse to the pocket center.
  4. This process is repeated until the programmed pocket depth is reached.

Finishing

  1. If finishing allowances have been defined, the control plunges and then approaches the contour. The approach movement occurs on a radius in order to ensure a gentle approach. The control first finishes the pocket walls, with multiple infeeds, if so specified.
  2. Then the control finishes the floor of the pocket from the inside out. The tool approaches the pocket floor tangentially

Notes

 
Notice
Danger of collision!
If you enter the depth in a cycle as a positive value, the control reverses the calculation of the pre-positioning. The tool moves at rapid traverse in the tool axis to set-up the clearance below the workpiece surface! There is a danger of collision!
  1. Enter depth as negative
  2. 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
 
Notice
Danger of collision!
If you call the cycle with machining operation 2 (only finishing), then the tool is positioned to the first plunging depth + set-up clearance at rapid traverse. There is a danger of collision during positioning at rapid traverse.
  1. Conduct a roughing operation beforehand
  2. 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.
  • At the end, the control returns the tool to set-up clearance, or to 2nd set-up clearance if one was programmed.
  • 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 251 takes the cutting width RCUTS from the tool table.
  • Plunging strategy Q366 with RCUTS

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 with radius compensation R0. Note parameter Q367 (position).
  • 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.
  • Please note that you need to define sufficiently large workpiece blank dimensions if Q224 Angle of rotation is not equal to 0.

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
Side finishing and floor finishing are executed only if the respective finishing allowance (Q368, Q369) has been defined

Input: 0, 1, 2

Q218 First side length?

Pocket length, parallel to the main axis of the working plane. This value has an incremental effect.

Input: 0...99999.9999

Q219 Second side length?

Pocket length, parallel to the secondary axis of the working plane. This value has an incremental effect.

Input: 0...99999.9999

Q220 Corner radius?

Radius of the pocket corner. If you have entered 0 here, the control assumes that the corner radius is equal to the tool radius.

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

Q224 Angle of rotation?

Angle by which the entire operation is rotated. The center of rotation is the position at which the tool is located when the cycle is called. This value has an absolute effect.

Input: –360.000...+360.000

Q367 Position of pocket (0/1/2/3/4)?

Position of the pocket with respect to the tool when the cycle is called:

0: Tool position = Center of pocket

1: Tool position = Lower left corner

2: Tool position = Lower right corner

3: Tool position = Upper right corner

4: Tool position = Upper left corner

Input: 0, 1, 2, 3, 4

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?

Q370 x tool radius = stepover factor k.

Input: 0.0001...1.41 or PREDEF

Q366 Plunging strategy (0/1/2)?

Type of plunging strategy:

0: Vertical plunging. The control plunges vertically, regardless of the plunging angle ANGLE defined in the tool table.

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.

2: Reciprocating plunge. 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. The reciprocation length depends on the plunging angle. As a minimum value, the control uses twice the tool diameter. If necessary, define the value of the RCUTS cutting width in the tool table.

PREDEF: The control uses the value from the GLOBAL DEF block

Input: 0, 1, 2 or PREDEF

Plunging strategy Q366 with RCUTS

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.

 
Tip

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.

Example

11 CYCL DEF 251 RECTANGULAR POCKET ~

Q215=+0

;MACHINING OPERATION ~

Q218=+60

;FIRST SIDE LENGTH ~

Q219=+20

;2ND SIDE LENGTH ~

Q220=+0

;CORNER RADIUS ~

Q368=+0

;ALLOWANCE FOR SIDE ~

Q224=+0

;ANGLE OF ROTATION ~

Q367=+0

;POCKET POSITION ~

Q207=+500

;FEED RATE MILLING ~

Q351=+1

;CLIMB OR UP-CUT ~

Q201=-20

;DEPTH ~

Q202=+5

;PLUNGING DEPTH ~

Q369=+0

;ALLOWANCE FOR FLOOR ~

Q206=+150

;FEED RATE FOR PLNGNG ~

Q338=+0

;INFEED FOR FINISHING ~

Q200=+2

;SET-UP CLEARANCE ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+50

;2ND SET-UP CLEARANCE ~

Q370=+1

;TOOL PATH OVERLAP ~

Q366=+1

;PLUNGE ~

Q385=+500

;FINISHING FEED RATE ~

Q439=+0

;FEED RATE REFERENCE

12 L X+50 Y+50 R0 FMAX M99

Plunging strategy Q366 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 is, 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

  • The control does not monitor or modify the helical path.

Reciprocating plunge Q366 = 2

RCUTS > 0

  • The control moves the tool along the complete reciprocating path.
  • If moving on a reciprocating path is not possible due to limited space, the control will display an error message.

RCUTS = 0 or undefined

  • The control moves the tool along one half of the reciprocating path.