Cycle 841 SIMPLE REC. TURNG., RADIAL DIR.

ISO programming

G841

Application

 
Machine

Refer to your machine manual.

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

This cycle enables you to recess right-angled slots in longitudinal direction. With recess turning, a recessing traverse to plunging depth and then a roughing traverse is alternatively machined. The machining process thus requires a minimum of retraction and infeed movements.

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 tool is outside the contour to be machined when the cycle is called, the cycle runs outside machining. If the tool is inside the contour to be machined, the cycle runs inside machining.

Related topics

  • Cycle 842 ENH.REC.TURNNG, RAD., optionally a chamfer or a rounding arc at the beginning or the end of a contour, angles for slot side walls and radii at the contour corners
  • Cycle 842 ENH.REC.TURNNG, RAD.

Roughing cycle sequence

The control uses the tool position as cycle starting point when the cycle is called. The cycle machines only the area from the cycle starting point to the end point defined in the cycle.

  1. From the cycle starting point, the control performs a recessing traverse until the first plunging depth is reached.
  2. The control machines the area between the starting position and the end point in longitudinal direction at the defined feed rate Q478.
  3. If the input parameter Q488 is defined in the cycle, plunging elements are machined at the programmed feed rate for plunging.
  4. 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.
  5. The tool recesses to the next plunging depth.
  6. The control repeats this procedure (steps 2 to 4) until the slot depth is reached.
  7. The control returns the tool to set-up clearance and performs a recessing traverse on both side walls.
  8. The control returns the tool at rapid traverse to the cycle starting point.

Finishing cycle sequence

  1. The control positions the tool at rapid traverse to the first slot side.
  2. The control finishes the side wall of the slot at the defined feed rate Q505.
  3. The control finishes the slot floor at the defined feed rate.
  4. The control retracts the tool at rapid traverse.
  5. The control positions the tool at rapid traverse to the second slot side.
  6. The control finishes the side wall of the slot at the defined feed rate Q505.
  7. The control returns the tool at rapid traverse to the cycle starting point.

Notes

  • This cycle can be executed only in the FUNCTION MODE TURN machining mode.
  • The tool position at cycle call (cycle start point) influences the area to be machined.
  • 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.

Note on programming

  • Program a positioning block to the starting 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

Q460 Set-up clearance?

Reserved; currently no functionality

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

Q478 Roughing feed rate?

Feed 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

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

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

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 841 SIMPLE REC. TURNG., RADIAL DIR. ~

Q215=+0

;MACHINING OPERATION ~

Q460=+2

;SAFETY CLEARANCE ~

Q493=+50

;DIAMETER AT CONTOUR END ~

Q494=-50

;CONTOUR END IN Z ~

Q478=+0.3

;ROUGHING FEED RATE ~

Q483=+0.4

;OVERSIZE FOR DIAMETER ~

Q484=+0.2

;OVERSIZE IN Z ~

Q505=+0.2

;FINISHING FEED RATE ~

Q463=+2

;MAX. CUTTING DEPTH ~

Q507=+0

;MACHINING DIRECTION ~

Q508=+0

;OFFSET WIDTH ~

Q509=+0

;DEPTH COMPENSATION ~

Q488=+0

;PLUNGING FEED RATE

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

13 CYCL CALL