Chamfer CHF

Application

The CHF chamfer function allows you to insert a chamfer between two straight lines. The size of the chamfer is based on the intersection that you have programmed with the straight lines.

Requirements

  • Straight lines in the working plane before and after the chamfer
  • Identical tool compensation before and after the chamfer
  • Chamfer is machinable with the current tool

Description of function

Cutting two straight lines creates contour corners. You can insert a chamfer at these contour corners. The angle of the corner is irrelevant; you simply define the length by which each straight line is shortened. The control does not traverse to the corner point.

If you program a feed rate in the CHF block, then this feed rate is in effect only while cutting the chamfer.

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 CHF 1 F200

; Chamfer with a size of 1 mm

To navigate to this function:

Insert NC function All functions Path contour CHF

The NC function includes the following syntax elements:

Syntax element

Meaning

CHF

Syntax initiator for a chamfer

1

Chamfer 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.

7 L X+0 Y+30 RL F300 M3

8 L X+40 IY+5

9 CHF 12 F250

10 L IX+5 Y+0