Curve Following Operations

The information in this section will help you create and edit Curve Following operations in your manufacturing program.

Select Curve Following then select the geometry to be machined

A number of strategy parameters are available for defining:

Specify the tool to be used , NC macros , and feeds and speeds as needed.

Curve Following Strategy Parameters

Curve Following: Machining Parameters

Tool path style
Indicates the cutting mode of the operation:
  • Zig Zag: the machining direction is reversed from one path to the next
  • One way: the same machining direction is used from one path to the next.
Machining tolerance
Specifies the maximum allowed distance between the theoretical and computed tool path.
Fixture accuracy
Specifies a tolerance applied to the fixture thickness. If the distance between the tool and fixture is less than fixture thickness minus fixture accuracy, the position is eliminated from the trajectory. If the distance is greater, the position is not eliminated.
Specifies the tool corrector identifier to be used in the operation.

The corrector type (P1, P2, P3, for example), corrector identifier and corrector number are defined on the tool. When the NC data source is generated, the corrector number can be generated using specific parameters.

Curve Following: Axial Stepover Parameters

Maximum depth of cut
Defines the maximum depth of cut in an axial strategy.
Number of levels
Defines the number of levels to be machined in an axial strategy.

Curve Following Geometry

You can specify the following Geometry:

Guiding contour can be specified in several ways:

Curve Following Tool

Most Milling and Drilling tool types can be used for Curve Following.

Curve Following Feeds and Speeds

In the Feeds and Speeds tab page, you can specify feedrates for approach, retract, and machining passes as well as a machining spindle speed.

Feedrates and spindle speed can be defined in linear or angular units.

A Spindle output checkbox is available for managing output of the SPINDL instruction in the generated NC data  file. If the checkbox is selected, the instruction is generated. Otherwise, it is not generated. 

Feeds and speeds of the operation can be updated automatically according to tooling data and the Rough or Finish quality of the operation. This is described in Update of Feeds and Speeds on Machining Operation.

Curve Following NC Macros

You can define transition paths in your machining operations by means of NC Macros. These transition paths are useful for providing approach, retract and linking motion in the tool path. 

An Approach macro is used to approach the operation start point.

A Retract macro is used to retract from the operation end point.

A Return between Levels macro is used in a multi-level machining operation to go to the next level.

A Clearance macro can be used in a machining operation to avoid a fixture, for example.