Continuous 5 Axis Activity Parameters

The Continuous 5 Axis Activity dialog box appears when you select Continuous 5 Axis Activity. The following parameters can be defined.

This page discusses:

See Also
In Other Guides
Generating Additive Activities

Tool Parameters

The Tools tab allows you to select an addditive tool.

Icon Description
Select a tool in the work area.
Edit local tool parameters.
Display additional resource information.

Geometry Parameters

The Geometry tab allows you to define geometries on the parts.

Mandatory

Parameter Description
Faces Selects the faces to be machined.
Start Guide Selects the start curve of the guide.
End Guide Selects the end curve of the guide.
Tool Axis Defines an axis for the trajectory.

To define the axis, two methods are available: using angular manipulators on a 3D representation of the tool, and a Tool Axis dialog box with the following parameters:

Parameter Description
Mode The possible values are:
  • Manual: lets you choose between the component and the angle
  • Selection: lets you select an existing geometric element
  • Feature Defined: retrieves the tool axis on an existing feature
  • Points in the view: lets you define an axis by clicking it in the view.
Components Lets you select the tool axis by defining the values on the X, Y and Z components.
Angle Lets you select the tool axis by defining an axis according to the reference tool axis.
Reverse Direction Lets you reverse the tool axis to make it point in the opposite direction to the one chosen in the component or angle.

Optional

Parameter Description
Tear Element A curve laying on the surface going from a point of the start guide to a point on the stop guide. The trajectory in a layer will start and stop at the Tear Element.

The Tear Element is only useful is the faces selected are forming a closed belt.
Border Guide 1 Selects the first edge where the trajectories of each layer will start or end.
Border Guide 2 Selects the second edge where the trajectories of each layer will start or end.

Strategy Parameters

The Strategy tab allows you to specify the strategy and user parameters.

Parameter Description
Tolerance Specifies the maximum deviation allowed between the design part and the manufactured part. By default, the value is 0.1m.
Helix's Pitch Defines the helix's pitch.
Radial Offset Defines the radial offset.
Technology Set Defines a set of values for all the technology parameters.

Tool Axis Parameters

The Tool Axis tab allows you to specify the tool axis mode, the collisions parameters and the kinematics checking.

Tool Axis Mode

Parameter Description
No 3/5 axis converter Enables or disables 3/5 axis converter availability.
Fixed Axis The tool axis arrow proposes a context menu:
  • Select: Defines the tool axis.
  • Analyze: Starts the Geometry Analyzer.
Thru a Point The tool axis passes through a specified point.
  • The label is a toggle to orient the tool axis To the point or From the point.
  • The point in the sensitive icon lets you select a point in the work area.
Thru a Guide The tool orientation is controlled by a geometrical curve (guide), that must be continuous. An open guide can be extrapolated at its extremities.
  • The label is a toggle to orient the tool axis To the guide or From the guide.
  • The red curve in the sensitive icon lets you select a curve in the work area.
  • Angle: Specifies a lead angle.
Normal to Part The tool axis is normal to the part.
Fixed Angle The new tool axis forms an angle with the initial tool axis.
  • Angle: Specifies this fixed angle.
  • Privileged angle with the tool path: Defines the angle a plane defined by the direction of motion (Frontal angle) or in a plane normal to the direction of motion (Lateral angle).
Normal to Drive Surface

The new tool axis is normal to the drive surface.

Angle: Specifies a possible lead angle.

Note: Use a smooth surface as the drive surface.

4 Axis Converts a 3-axis or 5-axis tool path as follows:
  • All the tool axes are tilted and constrained with a fixed angle with the normal (N) of the given reference plane.
  • All the tool axes are constrained along a cone defined by the angle with the normal of a reference plane (N) and a given point (P).
    Note: If the angle (Alpha) is defined as 90°, all the tool path axes are constrained to planes perpendicular to the normal of the given reference plane.
  • The associated parameter is Tilted/Cone angle. The Cone constraint check box lets you define a point to define the cone axis.

Collisions Checking

Parameter Description
Activate collisions checking Activates or deactivates collisions checking.
Collision checking strategy Defines the strategy: Automatic or Manual.
Part, Check, Design Part Enables collision checking on one or multiple elements.
Note: For collision checking with design parts, make sure that you have selected a valid Design Part in the Part Operation.
Fixtures (PO) Takes into account Check defined with the Part Operation
Additional Surface Selects additional surface to be checked.
Offset on Tool Defines the tolerance distance specific to the tool radius and tool length.
Offset on Tool Assembly Defines the tolerance distance specific to the tool assembly radius and tool length.
Max Discretization Angle Specifies the maximum angular change of tool axis between tool positions.
Minimum Length Specifies the minimum distance that must exist between two collision points to allow the modification of the tool axis between those two points.
Angle Mode Defines the angle mode: Frontal or Lateral.
Minimum Angle Defines the minimum angle range within which the tool axis can vary.
Maximum Angle Defines the maximum angle range within which the tool axis can vary.
Step Angle Defines the computation step used to find the optimal angle to avoid collisions. The smaller the Step Angle, the longer the computation time.

Macros Parameters

The Macros tab allows you to specify the macros to be used on the operation.

Macros Parameters

The Macros tab allows you to define transition paths in your machining operations by means of NC macros.

  • Approach
  • Retract

For more information, see NC Machining Apps Common Services: Using the Working Area: Creating Machining Operations: Defining Macros: NC Macros.

Feedrate Parameters

The Feedrate tab allows you to specify 3 different feedrates: approach feedrate, retract feedrate, or transition feedrate.

Table 1. Feedrates
Parameter Description
Approach Feedrate Defines the speed of linear advancement of the tool during its approach, before a fabrication motion. This parameter is applied when the machine is carrying out an approach motion.
Retract Feedrate Defines the speed of linear withdrawal of the tool during its regression. This parameter is applied when the machine is carrying out a retract motion.
Transition Feedrate Defines the speed of the tool when it is moving from the previous operation to the current one. It can be activated or not.