Cycle 204 BACK BORING

ISO programming

G204

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.

 
Tip

Special boring bars for upward cutting are required for this cycle.

This cycle allows counterbores to be machined from the underside of the workpiece.

Cycle sequence

  1. The control positions the tool in the spindle axis at rapid traverse FMAX to the specified set-up clearance above the workpiece surface
  2. The control then orients the spindle to the 0° position with an oriented spindle stop, and displaces the tool by the off-center distance.
  3. The tool is then plunged into the already bored hole at the feed rate for pre-positioning until the cutting edge has reached the programmed set-up clearance beneath the lower workpiece edge
  4. The control then centers the tool again in the bore hole, switches on the spindle and, if applicable, the coolant and moves the tool at the feed rate for counterboring to the depth programmed for the counterbore
  5. If programmed, the tool remains at the counterbore bottom. The tool will then be retracted from the hole again. The control carries out another oriented spindle stop and the tool is once again displaced by the off-center distance
  6. Finally the tool moves at FMAX to set-up clearance.
  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 necessary, the control moves the tool 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

Notes

 
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.
  • 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.
  • When calculating the starting point for boring, the control considers the cutting edge length of the boring bar and the thickness of the material.
  • 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 it is less than the DEPTH OF COUNTERBORE Q249, the control will display an error message.
 
Tip

Enter the tool length measured up to the lower edge of the boring bar, not the cutting edge.

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 cycle parameter depth determines the working direction. Note: If you enter a positive sign, the tool bores in the direction of the positive spindle axis.

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

Q249 Depth of counterbore?

Distance between underside of workpiece and the top of hole. A positive sign means the hole will be bored in the positive spindle axis direction. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q250 Material thickness?

Height of the workpiece. Enter an incremental value.

Input: 0.0001...99999.9999

Q251 Tool edge off-center distance?

Off-center distance of the boring bar. Refer to the tool data sheet. This value has an incremental effect.

Input: 0.0001...99999.9999

Q252 Tool edge height?

Distance between underside of boring bar and main cutting tooth. Refer to the tool data sheet. This value has an incremental effect.

Q253 Feed rate for pre-positioning?

Traversing speed of the tool in mm/min when plunging or when retracting.

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

Q254 Feed rate for counterboring?

Traversing speed of the tool in mm/min during counterboring

Input: 0...99999.999 or FAUTO, FU

Q255 Dwell time in secs.?

Dwell time in seconds at the bottom of the bore hole

Input: 0...99999

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 offsets the tool by the off-center distance (after orienting the spindle). Inputting 0 is not permitted

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: 1, 2, 3, 4

Q336 Angle for spindle orientation? (optional)

Angle at which the control positions the tool before it is plunged into or retracted from the bore hole This value has an absolute effect.

Input: 0...360

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 204 BACK BORING ~

Q200=+2

;SET-UP CLEARANCE ~

Q249=+2

;DEPTH OF COUNTERBORE ~

Q250=+20

;MATERIAL THICKNESS ~

Q251=+3.5

;OFF-CENTER DISTANCE ~

Q252=+15

;TOOL EDGE HEIGHT ~

Q253=+750

;F PRE-POSITIONING ~

Q254=+200

;F COUNTERBORING ~

Q255=+0

;DWELL TIME ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+50

;2ND SET-UP CLEARANCE ~

Q214=+0

;DISENGAGING DIRECTN ~

Q336=+0

;ANGLE OF SPINDLE