Cycle 24 SIDE FINISHING

ISO programming

G124

Application

Cycle 24 SIDE FINISHING allows you to finish your contour by taking the side finishing allowance into account that has been programmed in Cycle 20. You can run this cycle in climb or up-cut milling mode.

Before programming the call of Cycle 24, you need to program further cycles:

  • Cycle 14 CONTOUR or SEL CONTOUR
  • Cycle 20 CONTOUR DATA
  • Cycle 21 PILOT DRILLING, if applicable
  • Cycle 22 if required ROUGH-OUT

Cycle run

  1. The control positions the tool above the workpiece surface to the starting point for the approach position. This position in the plane results from a tangential arc on which the control moves the tool when approaching the contour
  2. The control then moves the tool to the first plunging depth using the feed rate for plunging
  3. The contour is approached on a tangential arc and machined up to the end. Each subcontour is finished separately
  4. The tool moves on a tangential helical arc when approaching the finishing contour or retracting from it. The starting height of the helix is 1/25 of the set-up clearance Q6, but max. the remaining last plunging depth above the final depth
  5. Finally, the tool retracts in the tool axis to the clearance height or to the position last programmed before the cycle. This behavior depends on the machine parameter posAfterContPocket (no. 201007).
 
Tip

The starting point calculated by the control also depends on the machining sequence. If you select the finishing cycle with the GOTO key and then start the NC program, the starting point can be at a different location from where it would be if you execute the NC program in the defined sequence.

Notes

 
Notice
Danger of collision!
If you have set the posAfterContPocket parameter (no. 201007) to ToolAxClearanceHeight, the control will position the tool at clearance height only in the direction of the tool axis when the cycle has finished. The control will not position the tool in the working plane. There is a danger of collision!
  1. After the end of the cycle, position the tool with all coordinates of the working plane (e.g., L X+80 Y+0 R0 FMAX)
  2. Make sure to program an absolute position after the cycle; do not program an incremental traversing movement
  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • If no finishing allowance was defined in Cycle 20, the control issues the error message Tool radius too large.
  • If you run Cycle 24 without having roughed out with Cycle 22, then enter "0" for the radius of the rough mill.
  • The control automatically calculates the starting point for finishing. The starting point depends on the available space in the pocket and the allowance programmed in Cycle 20.
  • If M110 is activated during operation, the feed rate for arcs compensated on the inside will be reduced accordingly.
  • This cycle monitors the defined usable length LU of the tool. If the LU value is less than the DEPTH Q15, the control will display an error message.
  • The cycle considers the miscellaneous functions M109 and M110. During the inside and outside machining of circular arcs the control keeps the feed rate constant at the cutting edge for inside and outside radii.
  • Adapting the feed rate for circular paths with M109

Notes on programming

  • The finishing allowance for the side Q14 is left over after finishing. Therefore, it must be smaller than the allowance in Cycle 20.
  • Cycle 24 can also be used for contour milling. In that case, you must do the following:
    • Define the contour to be milled as a single island (without pocket boundary)
    • In Cycle 20, enter a finishing allowance (Q3) greater than the sum of the finishing allowance Q14 + radius of the tool being used

Note regarding machine parameters

  • Use the machine parameter posAfterContPocket (no. 201007) to define how to move the tool after machining the contour pocket:
    • PosBeforeMachining: Return to starting position.
    • ToolAxClearanceHeight: Position the tool axis to clearance height.

Cycle parameters

Help graphic

Parameter

Q9 Direction of rotation? cw = -1

Machining direction:

+1: Counterclockwise

–1: Clockwise

Input: –1, +1

Q10 Plunging depth?

Tool infeed per cut. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q11 Feed rate for plunging?

Tool traversing speed in mm/min during plunging

Input: 0...99999.9999 or FAUTO, FU, FZ

Q12 Feed rate for roughing?

Traversing feed rate in the working plane

Input: 0...99999.9999 or FAUTO, FU, FZ

Q14 Finishing allowance for side?

The finishing allowance for the side Q14 is left over after finishing. This allowance must be smaller than the allowance in Cycle 20. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q438 or QS438 Number/name of rough-out tool?

Number or name of the tool that was used by the control to rough out the contour pocket. You are able to transfer the coarse roughing tool directly from the tool table via the action bar. In addition, you can enter the tool name via the Name in the action bar. The control automatically inserts the closing quotation mark when you exit the input field.

Q438 = –1: The control assumes that the tool last used is the rough-out tool (default behavior)

Q438 = 0: If there was no coarse-roughing, enter the number of a tool with the radius 0. This is usually the tool numbered 0.

Input: –1...+32767.9 or 255 characters

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 24 SIDE FINISHING ~

Q9=+1

;ROTATIONAL DIRECTION ~

Q10=+5

;PLUNGING DEPTH ~

Q11=+150

;FEED RATE FOR PLNGNG ~

Q12=+500

;FEED RATE F. ROUGHNG ~

Q14=+0

;ALLOWANCE FOR SIDE ~

Q438=-1

;ROUGH-OUT TOOL