Cycle 202 REAMING

ISO programming

G202

Application

 
Machine

Refer to your machine manual.

Machine and control must be specially prepared by the machine manufacturer for use of this cycle.

This cycle is effective only for machines with servo-controlled spindle.

With this cycle, you can bore holes. In this cycle, you can optionally define a dwell time at the bottom of the hole.

Cycle sequence

  1. The control positions the tool in the spindle axis at rapid traverse FMAX to the safety clearance Q200 above the workpiece Q203 SURFACE COORDINATE
  2. The tool drills to the programmed depth at the feed rate for plunging Q201
  3. If programmed, the tool remains at the hole bottom for the entered dwell time with active spindle rotation for cutting free.
  4. The control then carries out an oriented spindle stop to the position that is defined in the Q336 parameter
  5. If Q214 DISENGAGING DIRECTN is defined, the control retracts in the programmed direction by the value in CLEARANCE TO SIDE Q357
  6. Then the control moves the tool at the retraction feed rate Q208 to the set-up clearance Q200
  7. The tool is again centered in the hole
  8. The control restores the spindle status as it was at the cycle start.
  9. If programmed, the control moves the tool at FMAX to 2nd set-up clearance. The 2nd set-up clearance Q204 will only come into effect if its value is greater than the set-up clearance Q200. If Q214=0 the tool tip remains on the wall of the hole

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!
There is a risk of collision if you choose the wrong direction for retraction. Any mirroring performed in the working plane will not be taken into account for the direction of retraction. In contrast, the control will consider active transformations for retraction.
  1. Check the position of the tool tip when programming an oriented spindle stop with reference to the angle entered in Q336 (e.g., in the MDI application in the Manual operating mode). In this case, no transformations should be active.
  2. Select the angle so that the tool tip is parallel to the disengaging direction
  3. Choose a disengaging direction Q214 that moves the tool away from the wall of the hole.
 
Notice
Danger of collision!
If you have activated M136, the tool will not move to the programmed set-up clearance once the machining operation is finished. The spindle rotation will stop at the bottom of the hole which, in turn, also stops the feed motion. There is a danger of collision as the tool will not be retracted!
  1. Use M137 to deactivate M136 before the cycle start
  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • After machining, the control returns the tool to the starting point in the working plane. This way, you can continue positioning the tool incrementally.
  • If the M7 or M8 function was active before calling the cycle, the control will reconstruct this previous state at the end of 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.
  • If Q214 DISENGAGING DIRECTN is not 0, Q357 CLEARANCE TO SIDE is in effect.

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 boring

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 plunging applies.

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

Q214 Disengaging directn (0/1/2/3/4)?

Specify the direction in which the control retracts the tool at the hole bottom (after carrying out an oriented spindle stop)

0: Do not retract tool

1: Retract tool in negative main axis direction

2: Retract tool in negative secondary axis direction

3: Retract tool in positive main axis direction

4: Retract tool in positive secondary axis direction

Input: 0, 1, 2, 3, 4

Q336 Angle for spindle orientation? (optional)

Angle to which the control positions the tool before retracting it. This value has an absolute effect.

Input: 0...360

Q357 Safety clearance to the side? (optional)

Distance between tool tooth and the wall. This value has an incremental effect.

Only in effect if Q214 DISENGAGING DIRECTN is not 0.

Input: 0...99999.9999

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 202 BORING ~

Q200=+2

;SET-UP CLEARANCE ~

Q201=-20

;DEPTH ~

Q206=+150

;FEED RATE FOR PLNGNG ~

Q211=+0

;DWELL TIME AT DEPTH ~

Q208=+9999

;RETRACTION FEED RATE ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+50

;2ND SET-UP CLEARANCE ~

Q214=+0

;DISENGAGING DIRECTN ~

Q336=+0

;ANGLE OF SPINDLE ~

Q357=+0.2

;CLEARANCE TO SIDE

12 L X+30 Y+20 FMAX M3

13 CYCL CALL