Rounding RND

Application

The RND rounding arc function allows you to insert a rounding arc between two straight lines. The rounding arc is based on the intersection that you have programmed with the straight lines.

Requirements

  • Path functions before and after the rounding arc
  • Identical tool compensation before and after the rounding arc
  • Rounding is machinable with the current tool

Description of function

You program the rounding arc between two path functions. The circular arc connects tangentially to the previous and subsequent contour element. The control does not traverse to the intersection.

If you program a feed rate in the RND block, then this feed rate is in effect only while cutting the rounding arc.

Input

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.

11 RND R3 F200

; Radius with a size of 3 mm

To navigate to this function:

Insert NC function All functions Path contour RND

The NC function includes the following syntax elements:

Syntax element

Meaning

RND

Syntax initiator for a radius

R

Radius size

Number or numerical parameter

F, FAUTO

Feed rate

Feed rate F

Number or numerical parameter

Optional syntax element

Example

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.

5 L X+10 Y+40 RL F300 M3

6 L X+40 Y+25

7 RND R5 F100

8 L X+10 Y+5