Cycle 240 CENTERING

ISO programming

G240

Application

Use Cycle 240 CENTERING to machine center holes. You can specify the centering diameter or depth and an optional dwell time at the bottom. This dwell time is used for chip breaking at the bottom of the hole. If there is already a pilot hole then you can enter a deepened starting point.

Cycle sequence

  1. From the current position, the control positions the tool at rapid traverse FMAX in the working plane to the starting position.
  2. The control positions the tool at rapid traverse FMAX in the tool axis to the set-up clearance Q200 above the workpiece surface Q203.
  3. If you define Q342 ROUGHING DIAMETER not equal to 0, the control uses this value and the point angle of the tool T-ANGLE to calculate a deepened starting point. The control positions the tool at the F PRE-POSITIONING Q253 feed rate to the deepened starting point.
  4. The tool is centered at the programmed feed rate for plunging F to the programmed centering diameter or centering depth.
  5. If a dwell time Q211 is defined, the tool remains at the centering depth.
  6. Finally, the tool is retracted to the set-up clearance or to the 2nd set-up clearance at rapid traverse FMAX. The 2nd set-up clearance Q204 will only come into effect if its value is greater than the set-up clearance Q200.

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
  • This cycle monitors the defined usable length LU of the tool. If it is less than the machining depth, the control will display an error message.

Notes on programming

  • Program a positioning block to position the tool at the starting point (hole center) in the working plane with radius compensation R0.
  • The algebraic sign for the Q344 (diameter) or Q201 (depth) cycle parameter determines the working direction. If you program the diameter or 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

Q343 Select diameter/depth (1/0)

Select whether centering is based on the entered diameter or depth. If the control is to center based on the entered diameter, the point angle of the tool must be defined in the T-ANGLE column of the TOOL.T tool table.

0: Centering based on the entered depth

1: Centering based on the entered diameter

Input: 0, 1

Q201 Depth?

Distance between workpiece surface and centering bottom (tip of centering taper). Only effective if Q343=0 is defined. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q344 Diameter of counterbore

Centering diameter. Only effective if Q343=1 is defined.

Input: –99999.9999...+99999.9999

Q206 Feed rate for plunging?

Traversing speed of the tool in mm/min while centering

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

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?

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

Q342 Roughing diameter? (optional)

0: There is no hole

>0: Diameter of the pre-drilled hole

Input: 0...99999.9999

Q253 Feed rate for pre-positioning? (optional)

Traversing speed of the tool when approaching the deepened starting point. The speed is in mm/min.

Only in effect if Q342 ROUGHING DIAMETER is not 0.

Input: 0...99999.9999 or FMAX, FAUTO, 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.

 
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 240 CENTERING ~

Q200=+2

;SET-UP CLEARANCE ~

Q343=+1

;SELECT DIA./DEPTH ~

Q201=-2

;DEPTH ~

Q344=-10

;DIAMETER ~

Q206=+150

;FEED RATE FOR PLNGNG ~

Q211=+0

;DWELL TIME AT DEPTH ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+50

;2ND SET-UP CLEARANCE ~

Q342=+0

;ROUGHING DIAMETER ~

Q253=+750

;F PRE-POSITIONING