Cycle 232 FACE MILLING

ISO programming

G232

Application

With Cycle 232, you can face-mill a level surface in multiple infeeds while taking the finishing allowance into account. Three machining strategies are available:

  • Strategy Q389=0: Meander machining, stepover outside the surface being machined
  • Strategy Q389=1: Meander machining, stepover at the edge of the surface being machined
  • Strategy Q389=2: Line-by-line machining, retraction and stepover at the positioning feed rate

Cycle run

  1. From the current position, the control positions the tool at rapid traverse FMAX to the starting point 1 using positioning logic: If the current position in the spindle axis is further away from the workpiece than the 2nd set-up clearance, the control positions the tool first in the working plane and then in the spindle axis. Otherwise, it first moves it to 2nd set-up clearance and then in the working plane. The starting point in the working plane is offset from the edge of the workpiece by the tool radius and the set-up clearance to the side.
  2. The tool then moves in the spindle axis at the positioning feed rate to the first plunging depth calculated by the control.

Strategy Q389=0

  1. The tool subsequently advances at the programmed feed rate for milling to the end point 2. The end point lies outside the surface. The control calculates the end point from the programmed starting point, the programmed length, the programmed set-up clearance to the side and the tool radius.
  2. The control offsets the tool to the starting point in the next pass at the pre-positioning feed rate. The offset is calculated from the programmed width, the tool radius and the maximum path overlap factor.
  3. The tool then moves back in the direction of the starting point 1.
  4. The process is repeated until the programmed surface has been completed. At the end of the last pass, the tool plunges to the next machining depth.
  5. In order to avoid non-productive motions, the surface is then machined in reverse direction.
  6. The process is repeated until all infeeds have been machined. In the last infeed, simply the finishing allowance entered is milled at the finishing feed rate.
  7. At the end of the cycle, the tool is retracted at FMAX to the 2nd set-up clearance.

Strategy Q389=1

  1. The tool subsequently advances at the programmed feed rate for milling to the end point 2. The end point lies at the edge of the surface. The control calculates the end point from the programmed starting point, the programmed length and the tool radius.
  2. The control offsets the tool to the starting point in the next pass at the pre-positioning feed rate. The offset is calculated from the programmed width, the tool radius and the maximum path overlap factor.
  3. The tool then moves back in the direction of the starting point 1. The motion to the next pass again occurs at the edge of the workpiece.
  4. The process is repeated until the programmed surface has been completed. At the end of the last pass, the tool plunges to the next machining depth.
  5. In order to avoid non-productive motions, the surface is then machined in reverse direction.
  6. The process is repeated until all infeeds have been completed. In the last infeed, the programmed finishing allowance will be milled at the finishing feed rate.
  7. At the end of the cycle, the tool is retracted at FMAX to the 2nd set-up clearance.

Strategy Q389=2

  1. The tool subsequently advances at the programmed feed rate for milling to the end point 2. The end point lies outside the surface. The control calculates the end point from the programmed starting point, the programmed length, the programmed set-up clearance to the side and the tool radius.
  2. The control positions the tool in the spindle axis to the set-up clearance above the current infeed depth, and then moves it at the pre-positioning feed rate directly back to the starting point in the next pass. The control calculates the offset from the programmed width, the tool radius and the maximum path overlap factor.
  3. The tool then returns to the current infeed depth and moves in the direction of end point 2
  4. The process is repeated until the programmed surface has been machined completely. At the end of the last pass, the tool plunges to the next machining depth.
  5. In order to avoid non-productive motions, the surface is then machined in reverse direction.
  6. The process is repeated until all infeeds have been machined. In the last infeed, simply the finishing allowance entered is milled at the finishing feed rate.
  7. At the end of the cycle, the tool is retracted at FMAX to the 2nd set-up clearance.

Notes

  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.

Notes on programming

  • If you enter identical values for Q227 STARTNG PNT 3RD AXIS and Q386 END POINT 3RD AXIS, the control does not run the cycle (depth = 0 has been programmed).
  • Program Q227 greater than Q386. The control will otherwise display an error message.
 
Tip

Enter Q204 2ND SET-UP CLEARANCE in such a way that no collision with the workpiece or the fixtures can occur.

Cycle parameters

Help graphic

Parameter

Q389 Machining strategy (0/1/2)?

Define how the control will machine the surface:

0: Meander machining, stepover at positioning feed rate outside the surface to be machined

1: Meander machining, stepover at the feed rate for milling at the edge of the surface to be machined

2: Line-by-line machining, retraction and stepover at the positioning feed rate

Input: 0, 1, 2

Q225 Starting point in 1st axis?

Define the starting point coordinate of the surface to be machined in the main axis of the working plane. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q226 Starting point in 2nd axis?

Define the starting point coordinate of the surface to be machined in the secondary axis of the working plane. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q227 Starting point in 3rd axis?

Coordinate of the workpiece surface used to calculate the infeeds. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q386 End point in 3rd axis?

Coordinate in the spindle axis on which the surface will be face-milled. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q218 First side length?

Length of the surface to be machined in the main axis of the working plane. Use the algebraic sign to specify the direction of the first milling path referenced to the starting point in the 1st axis. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q219 Second side length?

Length of the surface to be machined in the secondary axis of the working plane. Use algebraic signs to specify the direction of the first cross feed referenced to the STARTNG PNT 2ND AXIS. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q202 Maximum plunging depth?

Maximum infeed per cut. The control calculates the actual plunging depth from the difference between the end point and starting point in the tool axis (taking the finishing allowance into account), so that uniform plunging depths are used each time. This value has an incremental effect.

Input: 0...99999.9999

Q369 Finishing allowance for floor?

Finishing allowance in depth which remains after roughing.

Input: 0...99999.9999

Q370 Max. path overlap factor?

Maximum stepover factor k. The control calculates the actual stepover from the second side length (Q219) and the tool radius so that a constant stepover is used for machining. If you have entered a radius R2 in the tool table (e.g., cutter radius when using a face-milling cutter), the control reduces the stepover accordingly.

Input: 0.001...1.999

Q207 Feed rate for milling?

Traversing speed of the tool in mm/min for milling

Input: 0...99999.999 or FAUTO, FU, FZ

Q385 Finishing feed rate?

Traversing speed of the tool in mm/min while milling the last infeed

Input: 0...99999.999 or FAUTO, FU, FZ

Q253 Feed rate for pre-positioning?

Traversing speed of the tool in mm/min when approaching the starting position and when moving to the next pass. If you are moving the tool transversely inside the material (Q389=1), the control uses the cross feed rate for milling Q207.

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

Q200 Set-up clearance?

Distance between tool tip and the starting position in the tool axis. If you are milling with machining strategy Q389 = 2, the control moves the tool to set-up clearance above the current plunging depth to the starting point of the next pass. This value has an incremental effect.

Input: 0...99999.9999 or PREDEF

Q357 Safety clearance to the side?

Parameter Q357 influences the following situations:

Approaching the first infeed depth: Q357 is the lateral distance from the tool to the workpiece.

Roughing with the Q389 = 0 to 3 roughing strategies: The surface to be machined is extended in Q350 MILLING DIRECTION by the value from Q357 if no limit has been set in that direction.

Side finishing: The paths are extended by Q357 in the Q350 MILLING DIRECTION.

Input: 0...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

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 232 FACE MILLING ~

Q389=+2

;STRATEGY ~

Q225=+0

;STARTNG PNT 1ST AXIS ~

Q226=+0

;STARTNG PNT 2ND AXIS ~

Q227=+2.5

;STARTNG PNT 3RD AXIS ~

Q386=0

;END POINT 3RD AXIS ~

Q218=+150

;FIRST SIDE LENGTH ~

Q219=+75

;2ND SIDE LENGTH ~

Q202=+5

;MAX. PLUNGING DEPTH ~

Q369=+0

;ALLOWANCE FOR FLOOR ~

Q370=+1

;MAX. OVERLAP ~

Q207=+500

;FEED RATE MILLING ~

Q385=+500

;FINISHING FEED RATE ~

Q253=+750

;F PRE-POSITIONING ~

Q200=+2

;SET-UP CLEARANCE ~

Q357=+2

;CLEARANCE TO SIDE ~

Q204=+50

;2ND SET-UP CLEARANCE