Cycle 850 RECESS TURNG, AXIAL

ISO programming

G850

Application

 
Machine

Refer to your machine manual.

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

cyc850

This cycle enables you to machine slots of any shape in transverse direction by recess turning. With recess turning, a recessing traverse to plunging depth and then a roughing traverse are alternatively performed.

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 coordinate of the contour starting point is larger than that of the contour end point, the cycle runs outside machining. If the coordinate of the contour starting point is less than that of the contour end point, 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 the contour starting point, the control positions the tool in the Z coordinate to the contour starting point and begins the cycle there.

  1. The control positions the tool at rapid traverse in the X coordinate (first recessing position).
  2. The control performs a recessing traverse until the first plunging depth is reached.
  3. The control machines the area between the starting position and the end point in transverse direction at the defined feed rate Q478.
  4. If the input parameter Q488 is defined in the cycle, plunging elements are machined at the programmed feed rate for plunging.
  5. If only one machining direction Q507=1 was specified in the cycle, the control lifts off the tool to the set-up clearance, retracts it at rapid traverse and approaches the contour again with the defined feed rate. With machining direction Q507=0, infeed is on both sides.
  6. The tool recesses to the next plunging depth.
  7. The control repeats this procedure (steps 2 to 4) until the slot depth is reached.
  8. The control returns the tool to set-up clearance and performs a recessing traverse on both side walls.
  9. The control returns the tool at rapid traverse to the cycle starting point.

Finishing cycle sequence

The control uses the position of the tool at cycle call as the cycle starting point.

  1. The control positions the tool at rapid traverse to the first slot side.
  2. The control finishes the side walls of the slot at the defined feed rate Q505.
  3. The control finishes the slot floor at the defined feed rate.
  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 defines the size of the area to be machined (cycle starting point)
  • From the second infeed, the control reduces each further traverse cutting movement by 0.1 mm. This reduces lateral pressure on the tool. If you specified an offset width Q508 for the cycle, the control reduces the cutting movement by this value. After pre-cutting, the remaining material is removed with a single cut. The control generates an error message if the lateral offset exceeds 80% of the effective cutting width (effective cutting width = cutter width – 2*cutting radius).
  • 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.

Notes on programming

  • Program a positioning block to the starting position with radius compensation R0 before the cycle call.
  • Before programming the cycle call, make sure to program Cycle 14 CONTOUR or SEL CONTOUR to be able to define the subprograms.
  • If you use local QL Q parameters in a contour subprogram, you must also assign or calculate these in the contour subprogram.

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

Q460 Set-up clearance?

Reserved; currently no functionality

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

Q488 Feed rate for plunging (0=auto)?

Definition of the feed rate during plunging. This input value is optional. If it is not programmed, then the feed rate defined for turning operations applies.

Input: 0...99999.999 or FAUTO

cyc850_2

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

Q479 Machining limits (0/1)?

Activate cutting limit:

0: No cutting limit active

1: Cutting limit (Q480/Q482)

Input: 0, 1

Q480 Value of diameter limit?

X value for contour limit (diameter value)

Input: –99999.999...+99999.999

Q482 Value of cutting limit in Z?

Z value for contour limit

Input: –99999.999...+99999.999

cyc850_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

Q507 Direction (0=bidir./1=unidir.)?

Cutting direction:

0: Bidirectional (in both directions)

1: Unidirectional (in direction of contour)

Input: 0, 1

Q508 Offset width?

Reduction of the cutting length. After pre-cutting, the remaining material is removed with a single cut. If required, the control limits the programmed offset width.

Input: 0...99.999

Q509 Depth compensat. for finishing?

Depending on the material, feed rate, etc., the tool tip is displaced during an operation. You can correct the resulting infeed error with the depth compensation factor.

Input: –9.9999...+9.9999

Q499 Reverse contour (0=no/1=yes)?

Machining direction:

0: Machining in the direction of contour

1: Machining in the direction opposite to the contour direction

Input: 0, 1

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 14.0 CONTOUR

12 CYCL DEF 14.1 CONTOUR LABEL2

13 CYCL DEF 850 RECESS TURNG, AXIAL ~

Q215=+0

;MACHINING OPERATION ~

Q460=+2

;SAFETY CLEARANCE ~

Q478=+0.3

;ROUGHING FEED RATE ~

Q488=0

;PLUNGING FEED RATE ~

Q483=+0.4

;OVERSIZE FOR DIAMETER ~

Q484=+0.2

;OVERSIZE IN Z ~

Q505=+0.2

;FINISHING FEED RATE ~

Q479=+0

;CONTOUR MACHINING LIMIT ~

Q480=+0

;DIAMETER LIMIT VALUE ~

Q482=+0

;LIMIT VALUE Z ~

Q463=+2

;MAX. CUTTING DEPTH ~

Q507=+0

;MACHINING DIRECTION ~

Q508=+0

;OFFSET WIDTH ~

Q509=+0

;DEPTH COMPENSATION ~

Q499=+0

;REVERSE CONTOUR

14 L X+75 Y+0 Z+2 R0 FMAX M303

15 CYCL CALL

16 M30

17 LBL 2

18 L X+60 Z+0

19 L Z-10

20 RND R5

21 L X+40 Y-15

22 L Z+0

23 LBL 0