Cycle 253 SLOT MILLING

ISO programming

G253

Application

Use Cycle 253 to completely machine a slot. 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. Starting from the left slot arc center, the tool moves in a reciprocating motion at the plunging angle defined in the tool table to the first infeed depth. Specify the plunging strategy with parameter Q366.
  2. The control roughs out the slot from the inside out, taking the finishing allowances (Q368 and Q369) into account
  3. The control retracts the tool to set-up clearance Q200. If the slot width matches the cutter diameter, the control retracts the tool from the slot after each infeed
  4. This process is repeated until the programmed slot depth is reached

Finishing

  1. If a finishing allowance has been defined during pre-machining, the control first finishes the slot walls, using multiple infeeds, if so specified. The slot wall is approached tangentially in the left slot arc
  2. Then the control finishes the floor of the slot from the inside out.

Notes

 
Notice
Danger of collision!
If you define a slot position not equal to 0, then the control only positions the tool in the tool axis to the 2nd set-up clearance. This means that the position at the end of the cycle does not have to correspond to the position at cycle start! There is a danger of collision!
  1. Do not program any incremental dimensions after this cycle
  2. Program an absolute position in all main axes after this cycle
 
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
  • 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.
  • If the slot width is greater than twice the tool diameter, the control roughs the slot correspondingly from the inside out. You can therefore mill any slots with small tools, too.
  • 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.
  • The control uses the RCUTS value in the cycle to monitor non-center-cut tools and to prevent the tool from front-face touching. If necessary, the control interrupts machining and issues an error message.

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.

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 Length of slot?

Enter the length of the slot. It is parallel to the main axis of the working plane. This value has an incremental effect.

Input: 0...99999.9999

Q219 Width of slot?

Enter the width of the slot, which must be parallel to the secondary axis of the working plane. If the slot width equals the tool diameter, the control will mill an oblong hole. This value has an incremental effect.

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

Q374 Angle of rotation?

Angle by which the entire slot 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 slot (0/1/2/3/4)?

Position of the figure relative to the position of the tool when the cycle is called:

0: Tool position = Center of figure

1: Tool position = Left end of figure

2: Tool position = Center of left figure arc

3: Tool position = Center of right figure arc

4: Tool position = Right end of figure

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 slot floor. 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

Q366 Plunging strategy (0/1/2)?

Type of plunging strategy:

0 = Vertical plunging. The plunging angle ANGLE in the tool table is not evaluated.

1, 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.

Alternative: PREDEF

Input: 0, 1, 2

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 253 SLOT MILLING ~

Q215=+0

;MACHINING OPERATION ~

Q218=+60

;SLOT LENGTH ~

Q219=+10

;SLOT WIDTH ~

Q368=+0

;ALLOWANCE FOR SIDE ~

Q374=+0

;ANGLE OF ROTATION ~

Q367=+0

;SLOT 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 ~

Q366=+2

;PLUNGE ~

Q385=+500

;FINISHING FEED RATE ~

Q439=+3

;FEED RATE REFERENCE

12 L X+50 Y+50 R0 FMAX M99