Recesses and undercuts

General information

Application

Some cycles machine contours that you have written in a subprogram. Further special contour elements are available to you for writing turning contours. In this way you can program recessing and undercutting as complete contour elements with a single NC block.

 
Tip

Recessing and undercutting are always referenced to a previously defined linear contour element.

Description of function

Various input options are available to you for defining undercuts and recesses. Some of these inputs have to be made (mandatory input); others can be skipped (optional input). The mandatory inputs are symbolized as such in the help graphics. In some elements, you can select between two different definitions. The control provides relevant selection possibilities via an action bar.

The control provides various possibilities for programming recesses and undercuts in the Recess / Undercut folder of the Insert NC function window.

Programming recessing

Recessing is the machining of recesses into round parts, usually for accommodation of locking rings and seals, or as lubricating grooves. You can program recessing around the circumference or on the face end of the turned part. You have two separate contour elements for this purpose:

  • GRV RADIAL: Recess in circumference of component
  • GRV AXIAL: Recess on face end of component
Input parameters in recessing GRV

Parameter

Meaning

Input

CENTER

Center of recess

Required

R

Corner radius of both inside corners

Optional

DEPTH / DIAM

Depth of recess (pay attention to algebraic sign!) /diameter of recess base

Required

BREADTH

Recess width

Required

ANGLE / ANG_WIDTH

Flank angle / opening angle between both flanks

Optional

RND / CHF

Rounding / chamfer on contour corner near to starting point

Optional

FAR_RND / FAR_CHF

Rounding / chamfer on contour corner away from starting point

Optional

 
Tip

The algebraic sign for the recess depth specifies the machining position (inside/outside machining) of the recess.

Algebraic signs of recess depth for outside machining:

  • If the contour element is in the negative direction of the Z coordinate, use a negative sign
  • If the contour element is in the positive direction of the Z coordinate, use a positive sign

Algebraic signs of recess depth for inside machining:

  • If the contour element is in the negative direction of the Z coordinate, use a positive sign
  • If the contour element is in the positive direction of the Z coordinate, use a negative sign

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: Radial recess with depth = 5, width = 10, pos. = Z-15

11 L X+40 Z+0

12 L Z-30

13 GRV RADIAL CENTER-15 DEPTH-5 BREADTH10 CHF1 FAR_CHF1

14 L X+60

Programming undercutting

Undercutting is usually required for the flush connection of components. In addition, undercutting can help reduce the notch effect at corners. Threads and fits are often machined with an undercut. You have various contour elements for defining the different undercuts:

  • UDC TYPE_E: Undercut for cylindrical surfaces to be further processed as per DIN 509.
  • UDC TYPE_F: Undercut for plane surface and cylindrical surface to be further processed as per DIN 509
  • UDC TYPE_H: Undercut for more rounded transition as per DIN 509
  • UDC TYPE_K: Undercut in plane surface and cylindrical surface
  • UDC TYPE_U: Undercut in cylindrical surface
  • UDC THREAD: Thread undercut as per DIN 76
 
Tip

The control always interprets undercuts as form elements in the longitudinal direction. No undercuts are possible in the plane direction.

Undercut DIN 509 UDC TYPE _E

Input parameters in undercut DIN 509 UDC TYPE_E

Parameter

Meaning

Input

R

Corner radius of both inside corners

Optional

DEPTH

Undercut depth

Optional

BREADTH

Width of undercut

Optional

ANGLE

Undercut angle

Optional

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: Undercut with depth = 2, width = 15

11 L X+40 Z+0

12 L Z-30

13 UDC TYPE_E R1 DEPTH2 BREADTH15

14 L X+60

Undercut DIN 509 UDC TYPE_F

Input parameters in undercut DIN 509 UDC TYPE_F

Parameter

Meaning

Input

R

Corner radius of both inside corners

Optional

DEPTH

Undercut depth

Optional

BREADTH

Width of undercut

Optional

ANGLE

Undercut angle

Optional

FACEDEPTH

Depth of face

Optional

FACEANGLE

Contour angle of face

Optional

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: Undercut form F with depth = 2, width = 15, depth of face = 1

11 L X+40 Z+0

12 L Z-30

13 UDC TYPE_F R1 DEPTH2 BREADTH15 FACEDEPTH1

14 L X+60

Undercut DIN 509 UDC TYPE_H

Input parameters in undercut DIN 509 UDC TYPE_H

Parameter

Meaning

Input

R

Corner radius of both inside corners

Required

BREADTH

Width of undercut

Required

ANGLE

Undercut angle

Required

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: Undercut form H with depth = 2, width = 15, angle = 10°

11 L X+40 Z+0

12 L Z-30

13 UDC TYPE_H R1 BREADTH10 ANGLE10

14 L X+60

Undercut UDC TYPE_K

Input parameters in undercut UDC TYPE_K

Parameter

Meaning

Input

R

Corner radius of both inside corners

Required

DEPTH

Undercut depth (parallel to axis)

Required

ROT

Angle relative to longitudinal axis (default: 45°)

Optional

ANG_WIDTH

Angle of undercut opening

Required

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: Undercut form K with depth = 2, width = 15, opening angle = 30°

11 L X+40 Z+0

12 L Z-30

13 UDC TYPE_K R1 DEPTH3 ANG_WIDTH30

14 L X+60

Undercut UDC TYPE_U

Input parameters in undercut UDC TYPE_U

Parameter

Meaning

Input

R

Corner radius of both inside corners

Required

DEPTH

Undercut depth

Required

BREADTH

Width of undercut

Required

RND / CHF

Rounding / chamfer on outside corner

Required

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: Undercut form U with depth = 3, width = 8

11 L X+40 Z+0

12 L Z-30

13 UDC TYPE_U R1 DEPTH3 BREADTH8 RND1

14 L X+60

Undercut UDC THREAD

Input parameters in undercut DIN 76 UDC THREAD

Parameter

Meaning

Input

PITCH

Thread pitch

Optional

R

Corner radius of both inside corners

Optional

DEPTH

Undercut depth

Optional

BREADTH

Width of undercut

Optional

ANGLE

Undercut angle

Optional

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: Thread undercut according to DIN 76 with thread pitch = 2

11 L X+40 Z+0

12 L Z-30

13 UDC THREAD PITCH2

14 L X+60