Cycle 233 FACE MILLING

ISO programming

G233

Application

With Cycle 233, you can face-mill a level surface in multiple infeeds while taking the finishing allowance into account. You can also define side walls in the cycle, which are then taken into account when machining the level surface. The cycle offers you various machining strategies:

  • 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: The surface is machined line by line with overtravel; stepover when retracting at rapid traverse
  • Strategy Q389=3: The surface is machined line by line without overtravel; stepover when retracting at rapid traverse
  • Strategy Q389=4: Helical machining from the outside toward the inside

Strategies Q389=0 and Q389 =1

The strategies Q389=0 and Q389=1 differ in the overtravel during face milling. If Q389=0, the end point lies outside of the surface, with Q389=1, it lies at the edge of the surface. The control calculates end point 2 from the side length and the set-up clearance to the side. If the strategy Q389=0 is used, the control additionally moves the tool beyond the level surface by the tool radius.

Cycle sequence

  1. From the current position, the control positions the tool at rapid traverse FMAX to the starting point 1 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 control then positions the tool at rapid traverse FMAX to set-up clearance in the spindle axis.
  3. The tool then moves in the spindle axis at the feed rate for milling Q207 to the first plunging depth calculated by the control.
  1. The control moves the tool to end point 2 at the programmed feed rate for milling.
  2. The control then shifts the tool laterally to the starting point of the next line at the pre-positioning feed rate. The control calculates the offset from the programmed width, the tool radius, the maximum path overlap factor and the set-up clearance to the side.
  3. The tool then returns in the opposite direction at the feed rate for milling.
  4. The process is repeated until the programmed surface has been machined completely.
  5. The control then positions the tool at rapid traverse FMAX back to starting point 1.
  6. If more than one infeed is required, the control moves the tool in the spindle axis to the next plunging depth at the positioning feed rate.
  7. 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.
  8. At the end of the cycle, the tool is retracted at FMAX to the 2nd set-up clearance.

Strategies Q389=2 and Q389 =3

The strategies Q389=2 and Q389=3 differ in the overtravel during face milling. If Q389=2, the end point lies outside of the surface, with Q389=3, it lies at the edge of the surface. The control calculates end point 2 from the side length and the set-up clearance to the side. If the strategy Q389=2 is used, the control additionally moves the tool beyond the level surface by the tool radius.

Cycle sequence

  1. From the current position, the control positions the tool at rapid traverse FMAX to the starting point 1 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 control then positions the tool at rapid traverse FMAX to set-up clearance in the spindle axis.
  3. The tool then moves in the spindle axis at the feed rate for milling Q207 to the first plunging depth calculated by the control.
  1. The tool subsequently advances at the programmed feed rate for milling Q207 to the end point 2.
  2. The control positions the tool in the tool axis to the set-up clearance above the current infeed depth, and then moves at FMAX directly back to the starting point in the next pass. The control calculates the offset from the programmed width, the tool radius, the maximum path overlap factor Q370 and the set-up clearance to the side Q357.
  3. The tool then returns to the current infeed depth and moves in the direction of the end point 2.
  4. The process is repeated until the programmed surface has been machined completely. At the end of the last path, the control returns the tool at rapid traverse FMAX to starting point 1.
  5. If more than one infeed is required, the control moves the tool in the spindle axis to the next plunging depth at the positioning feed rate.
  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.

Strategies Q389=2 and Q389=3—with lateral limitation

If you program a lateral limitation, the control might not be able to perform movements outside of the contour. In this case the cycle runs as follows:

  1. The control positions the tool at FMAX to the starting point in the working plane. This position is offset from the edge of the workpiece by the tool radius and the set-up clearance Q357 to the side.
  2. The tool moves at rapid traverse FMAX in the tool axis to the set-up clearance Q200 and from there at Q207 FEED RATE MILLING to the first plunging depth Q202.
  3. The control moves the tool on a circular path to the starting point 1.
  4. The tool moves at the programmed feed rate Q207 to the end point 2 and departs from the contour on a circular path.
  5. Then the control moves the tool to the approach position of the next path at Q253 F PRE-POSITIONING.
  6. Steps 3 to 5 are repeated until the entire surface is milled.
  7. If more than one infeed depth is programmed, the control moves the tool at the end of the last path to the set-up clearance Q200 and positions in the working plane to the next approach position.
  8. In the last infeed the control mills the Q369 ALLOWANCE FOR FLOOR at Q385 FINISHING FEED RATE.
  9. At the end of the last path, the control retracts the tool to the 2nd set-up clearance Q204 and then to the position last programmed before the cycle.
  10.  
    Tip
    • The circular paths for approaching and departing the paths depend on Q220 CORNER RADIUS.
    • The control calculates the offset from the programmed width, the tool radius, the maximum path overlap factor Q370 and the set-up clearance to the side Q357.

Strategy Q389=4

Cycle sequence

  1. From the current position, the control positions the tool at rapid traverse FMAX to the starting point 1 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 control then positions the tool at rapid traverse FMAX to set-up clearance in the spindle axis.
  3. The tool then moves in the spindle axis at the feed rate for milling Q207 to the first plunging depth calculated by the control.
  1. The tool subsequently moves to the starting point of the milling path at the programmed Feed rate for milling on a tangential approach path.
  2. The control machines the level surface at the feed rate for milling from the outside toward the inside with ever-shorter milling paths. The constant stepover results in the tool being continuously engaged.
  3. The process is repeated until the programmed surface has been completed. At the end of the last path, the control returns the tool at rapid traverse FMAX to starting point 1.
  4. If more than one infeed is required, the control moves the tool in the spindle axis to the next plunging depth at the positioning feed rate.
  5. 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.
  6. At the end of the cycle, the tool is retracted at FMAX to the 2nd set-up clearance.

Limits

The limits enable you to set limits to the machining of the level surface so that, for example, side walls or shoulders are considered during machining. A side wall that is defined by a limit is machined to the finished dimension resulting from the starting point or the side lengths of the level surface. During roughing the control takes the allowance for the side into account, whereas during finishing the allowance is used for pre-positioning the tool.

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 can be executed only in the FUNCTION MODE MILL machining mode.
  • The control automatically pre-positions the tool in the tool axis. Make sure to program Q204 2ND SET-UP CLEARANCE correctly.
  • The control reduces the plunging depth to the LCUTS cutting edge length defined in the tool table if the cutting edge length is shorter than the Q202 plunging depth programmed in the cycle.
  • Cycle 233 monitors the entries made for the tool or cutting edge length in LCUTS in the tool table. If the tool or cutting edge length is not sufficient for a finishing operation, the control will subdivide the process into multiple machining steps.
  • 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.
  • This cycle finishes Q369 ALLOWANCE FOR FLOOR with only one infeed. Parameter Q338 INFEED FOR FINISHING has no effect on Q369. Q338 is effective in finishing of Q368 ALLOWANCE FOR SIDE.

Notes on programming

  • Pre-position the tool in the working plane to the starting position with radius compensation R0. Note the machining direction.
  • 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).
  • If you define Q370 TOOL PATH OVERLAP >1, the programmed overlap factor will be taken into account right from the first machining path.
  • If a limit (Q347, Q348 or Q349) was programmed in the machining direction Q350, the cycle will extend the contour in the infeed direction by corner radius Q220. The specified surface will be machined completely.
 
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

Q215 Machining operation (0/1/2)?

Define the machining operation:

0: Roughing and finishing

1: Only roughing

2: Only finishing
Side finishing and floor finishing are executed only if the respective finishing allowance (Q368, Q369) has been defined

Input: 0, 1, 2

Q389 Machining strategy (0-4)?

Specify how the control machines 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: Machining line by line, retraction and stepover at positioning feed rate outside the surface to be machined

3: Machining line by line, retraction and stepover at positioning feed rate at the edge of the surface to be machined

4: Helical machining, uniform infeed from the outside toward the inside

Input: 0, 1, 2, 3, 4

Q350 Milling direction?

Axis in the working plane that defines the machining direction:

1: Main axis = Machining direction

2: Secondary axis = Machining direction

Input: 1, 2

Q218 First side length?

Length of the surface to be machined in the main axis of the working plane, referencing 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

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

Q369 Finishing allowance for floor?

Finishing allowance in depth which remains after roughing.

This value has an incremental effect.

Input: 0...99999.9999

Q202 Maximum plunging depth?

Infeed per cut. Enter an incremental value greater than 0.

Input: 0...99999.9999

Q370 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.

Input: 0.0001...1.9999

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

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.

This value has an incremental effect.

Input: 0...99999.9999

Q200 Set-up clearance?

Distance between tool tip and workpiece surface. This value has an incremental effect.

Input: 0...99999.9999 or PREDEF

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

Q347 1st limit?

Select the side of the workpiece where the plane surface is bordered by a side wall (not possible with helical machining). Depending on the position of the side wall, the control limits the machining of the plane surface to the corresponding starting point coordinate or side length:

0: No limitation

-1: Limit in negative main axis

+1: Limit in positive main axis

-2: Limit in negative secondary axis

+2: Limit in positive secondary axis

Input: –2, –1, 0, +1, +2

Q348 2nd limit?

See parameter Q347 1st limit

Input: –2, –1, 0, +1, +2

Q349 3rd limit?

See parameter Q347 1st limit

Input: –2, –1, 0, +1, +2

Q220 Corner radius?

Radius of a corner at limits (Q347 to Q349)

Input: 0...99999.9999

Q368 Finishing allowance for side?

Finishing allowance in the machining plane which remains after roughing. This value has an incremental effect.

Input: 0...99999.9999

Q338 Infeed for finishing?

Infeed in the tool axis when finishing the lateral finishing allowance Q368. This value has an incremental effect.

0: Finishing in one infeed

Input: 0...99999.9999

Q367 Surface position (-1/0/1/2/3/4)? (optional)

Position of the surface relative to the position of the tool when the cycle is called:

-1: Tool position = Current position

0: Tool position = Center of stud

1: Tool position = Lower left corner

2: Tool position = Lower right corner

3: Tool position = Upper right corner

4: Tool position = Upper left corner

Input: –1, 0, +1, +2, +3, +4

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 233 FACE MILLING ~

Q215=+0

;MACHINING OPERATION ~

Q389=+2

;MILLING STRATEGY ~

Q350=+1

;MILLING DIRECTION ~

Q218=+60

;FIRST SIDE LENGTH ~

Q219=+20

;2ND SIDE LENGTH ~

Q227=+0

;STARTNG PNT 3RD AXIS ~

Q386=+0

;END POINT 3RD AXIS ~

Q369=+0

;ALLOWANCE FOR FLOOR ~

Q202=+5

;MAX. PLUNGING DEPTH ~

Q370=+1

;TOOL PATH OVERLAP ~

Q207=+500

;FEED RATE MILLING ~

Q385=+500

;FINISHING FEED RATE ~

Q253=+750

;F PRE-POSITIONING ~

Q357=+2

;CLEARANCE TO SIDE ~

Q200=+2

;SET-UP CLEARANCE ~

Q204=+50

;2ND SET-UP CLEARANCE ~

Q347=+0

;1ST LIMIT ~

Q348=+0

;2ND LIMIT ~

Q349=+0

;3RD LIMIT ~

Q220=+0

;CORNER RADIUS ~

Q368=+0

;ALLOWANCE FOR SIDE ~

Q338=+0

;INFEED FOR FINISHING ~

Q367=-1

;SURFACE POSITION

12 L X+50 Y+50 R0 FMAX M99