Cycle 814 TURN PLUNGE LONGITUDINAL EXT.

ISO programming

G814

Application

 
Machine

Refer to your machine manual.

This function must be enabled and adapted by the machine manufacturer.

cyc814

This cycle enables you to run longitudinal turning of shoulders with plunging elements (undercuts). Extended scope of function:

  • You can insert a chamfer or curve at the contour start and contour end.
  • In the cycle you can define an angle for the face and a radius for the contour edge

You can use the cycle either for roughing, finishing or complete machining. Turning is run paraxially with roughing.

The cycle can be used for inside and outside machining. If the start diameter Q491 is larger than the end diameter Q493, the cycle runs outside machining. If the start diameter Q491 is less than the end diameter Q493, the cycle runs inside machining.

Roughing cycle sequence

The control uses the tool position as cycle starting point when the cycle is called. If the Z coordinate of the starting point is less than Q492 Contour start in Z, the control positions the tool in the Z coordinate to set-up clearance and begins the cycle there.

In undercutting, the control uses feed rate Q478 for the infeed. The control always retracts the tool to the set-up clearance.

  1. The control performs a paraxial infeed movement at rapid traverse. The control calculates the infeed value based on Q463 Maximum cutting depth.
  2. The control machines the area between the starting position and the end point in longitudinal direction at the defined feed rate Q478.
  3. The control retracts the tool at the defined feed rate by the infeed value.
  4. The control returns the tool at rapid traverse to the beginning of cut.
  5. The control repeats this procedure (steps 1 to 4) until the contour is completed.
  6. The control returns the tool at rapid traverse to the cycle starting point.

Finishing cycle sequence

  1. The infeed movement is performed at rapid traverse.
  2. The control finishes the contour of the finished part (contour starting point to contour end point) at the defined feed rate Q505.
  3. The control retracts the tool at the defined feed rate to the set-up clearance.
  4. The control returns the tool at rapid traverse to the cycle starting point.

Notes

  • This cycle can only be executed in the FUNCTION MODE TURN machining mode.
  • The tool position at cycle call (cycle start point) influences the area to be machined.
  • The control takes the cutting geometry of the tool into account to prevent damage to contour elements. If it is not possible to machine the entire workpiece with the active tool, the control will display a warning.
  • If you programmed a value for CUTLENGTH, then it will be taken into account during the roughing operation in this cycle. A message is displayed and the plunging depth is automatically reduced.
  • Also refer to the fundamentals of the turning cycles.
  • Fundamentals of turning cycles

Note on programming

  • Program a positioning block to a safe position with radius compensation R0 before the cycle call.

Cycle parameters

Help graphic

Parameter

Q215 Machining operation (0/1/2/3)?

Define extent of machining:

0: Roughing and finishing

1: Only roughing

2: Only finishing to final dimension

3: Only finishing to oversize

Input: 0, 1, 2, 3

cyc814_1

cyc814_2

Q460 Set-up clearance?

Distance for retraction and prepositioning. This value has an incremental effect.

Input: 0...999.999

Q491 Diameter at contour start?

X coordinate of the contour starting point (diameter value)

Input: –99999.999...+99999.999

Q492 Contour start in Z?

Z coordinate of the starting point for the plunging path

Input: –99999.999...+99999.999

Q493 Diameter at end of contour?

X coordinate of the contour end point (diameter value)

Input: –99999.999...+99999.999

Q494 Contour end in Z?

Z coordinate of the contour end point

Input: –99999.999...+99999.999

Q495 Angle of side?

Angle of plunging flank. The reference angle is the line perpendicular to the rotary axis.

Input: 0...89.9999

Q501 Starting element type (0/1/2)?

Define the type of element at the beginning of the contour (circumferential surface):

0: No additional element

1: Element is a chamfer

2: Element is a radius

Input: 0, 1, 2

Q502 Size of starting element?

Size of the starting element (chamfer section)

Input: 0...999.999

Q500 Radius of the contour corner?

Radius of the inside corner of the contour. If no radius is specified, the radius will be that of the indexable insert.

Input: 0...999.999

Q496 Angle of face?

Angle between the plane surface and the rotary axis

Input: 0...89.9999

Q503 End element type (0/1/2)?

Define the type of element at the contour end (plane surface):

0: No additional element

1: Element is a chamfer

2: Element is a radius

Input: 0, 1, 2

Q504 Size of end element?

Size of the end element (chamfer section)

Input: 0...999.999

cyc814_1

Q463 Maximum cutting depth?

Maximum infeed (radius value) in the radial direction. The infeed is distributed evenly to avoid abrasive cuts.

Input: 0...99.999

Q478 Roughing feed rate?

Freed rate during roughing. If M136 has been programmed, the value is interpreted by the control in millimeters per revolution; without M136, in millimeters per minute.

Input: 0...99999.999 or FAUTO

Q483 Oversize for diameter?

Diameter oversize on the defined contour. This value has an incremental effect.

Input: 0...99.999

Q484 Oversize in Z?

Oversize of the defined contour in the axial direction. This value has an incremental effect.

Input: 0...99.999

Q505 Finishing feed rate?

Feed rate during finishing. If M136 has been programmed, the value is interpreted by the control in millimeters per revolution; without M136, in millimeters per minute.

Input: 0...99999.999 or FAUTO

Q506 Contour smoothing (0/1/2)?

0: Along the contour after every cut (within the infeed area)

1: Contour smoothing after the last cut (entire contour); retract by 45°

2: No contour smoothing; retract by 45°

Input: 0, 1, 2

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 814 TURN PLUNGE LONGITUDINAL EXT. ~

Q215=+0

;MACHINING OPERATION ~

Q460=+2

;SAFETY CLEARANCE ~

Q491=+75

;DIAMETER AT CONTOUR START ~

Q492=-10

;CONTOUR START IN Z ~

Q493=+50

;DIAMETER AT CONTOUR END ~

Q494=-55

;CONTOUR END IN Z ~

Q495=+70

;ANGLE OF SIDE ~

Q501=+1

;TYPE OF STARTING ELEMENT ~

Q502=+0.5

;SIZE OF STARTING ELEMENT ~

Q500=+1.5

;RADIUS OF CONTOUR EDGE ~

Q496=+0

;ANGLE OF FACE ~

Q503=+1

;TYPE OF END ELEMENT ~

Q504=+0.5

;SIZE OF END ELEMENT ~

Q463=+3

;MAX. CUTTING DEPTH ~

Q478=+0.3

;ROUGHING FEED RATE ~

Q483=+0.4

;OVERSIZE FOR DIAMETER ~

Q484=+0.2

;OVERSIZE IN Z ~

Q505=+0.2

;FINISHING FEED RATE ~

Q506=+0

;CONTOUR SMOOTHING

12 L X+75 Y+0 Z+2 FMAX M303

13 CYCL CALL