Curve Following

The Curve Following dialog box appears when you select Curve Following. This dialog box contain controls for:

Related Topics
Creating a Curve Following Operation



Machining Strategy Parameters



Tool path style
Specifies tool path style.

The options in the Tool path style dropdown combo box are as follows:

  • 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 Parameters



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.
Compensation
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.

Axial 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.

User Parameters

See Adding an User Parameter

Geometry



You can specify the following geometry:

  • Guiding contour (edges or sketch) with possibleAxial Offset.

    Note: this must be a continuous contour.

  • Check elements with possible Offset on Check.

Tools

Most milling and drilling tool types can be used for Curve Following.

See Specifying a Tool Element in a Machining Operation

Feedrates and Speeds Parameters



Feedrate: Automatic compute from tooling Feeds and Speeds
This check box allow an operation's feeds and speeds values to be updated automatically when the tool's feeds and speeds values are modified.

You can specify the following feedrates:

  • Approach
  • Machining
  • Retract
  • Finishing

Note:

The above feedrates can be defined in linear (feed per minute) or angular (feed per revolution) units.

  • Angular: feedrate in revolutions per minute and unit is set to mm_turn.
  • Linear: feedrate in feed per minute and unit is set to mm_mn.

Transition
You can locally set the feedrate for a transition path to a machining operation B from a machining operation A or from a tool change activity. This is done by selecting the Transition check box in the Machining Operation dialog box for operation B.

For more information, please refer to the Setting a Transition Feedrate.

Spindle Speed: Automatic compute from tooling Feeds and Speeds

This check box allow an operation's feeds and speeds values to be updated automatically when the tool's feeds and speeds values are modified.

If the Feedrate Automatic compute check box is selected and the Spindle Speed: Automatic compute from tooling Feeds and Speeds check box is not selected, then only the feedrate values can be computed. If both are not selected then automatic updating is not done.

When you modify a tool's feeds and speeds, all existing operations with the Automatic compute check boxes selected that use this tool (or an assembly using this tool) can be recomputed.

Spindle output
This check box manage output of the SPINDL instruction in the generated NC data file:
  • If the check box is selected, the instruction is generated.
  • Otherwise, it is not generated.

Note:

Spindle speed is applied on the different motions of the operations (including approach, retract, linking macros). Spindle can be re-defined with Spindle tool motion. The spindle speed can be defined in linear (length per minute) or angular (length per revolution) units.

  • Angular: length in revolutions per minute and unit is set to mm_turn.
  • Linear: length in feed per minute and unit is set to mm_mn.

Quality
The feed and speed values are computed according to the Quality setting on the operation.
Compute
Feeds and speeds of the operation can be updated according to tooling feeds and speeds by clicking the Compute button located in the Feeds and Speeds tab of the operation.

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 About Feeds and Speeds.

NC Macros



You can define transition paths in your machining operations by means of NC macros:

  • Approach: to approach the operation start point,
  • Retract: to retract from the operation end point,
  • Return between Levels to go to the next level in a multi-level machining operation,
  • Clearance to avoid a fixture, for example.

The proposed macro mode for Approach and Retract macro are:

  • None
  • Build by user
  • Horizontal horizontal axial
  • Axial
  • Ramping

The proposed macro mode for Clearance macro are:

  • Distance
  • To a Plane
  • To safety plane

For more information, please refer to the Defining Macros.