4-Axis Curve Sweeping

The 4-Axis Curve Sweeping dialog box appears when you select 4-Axis Curve Sweeping from the Surface Machining section.

This dialog box contains controls for:

This page discusses:

See Also
Creating a 4-Axis Curve Sweeping Operation

Resource Parameters

The Resource tab allows you to select a tool.

Resource Tab
Parameter Description
Select a Tool from Session Selects a tool in Resource Configuration View.
Select from Catalog Selects a tool from a reference tool file or PLM catalog.
Select from Database Selects a tool from the database.
Display Tool Properties Accesses tool parameters.
Define Tool Axis Defines the tool axis.
Tool Number Defines the number of tools.
Display Tool Displays the tool position.
Default Displays the tool at default position.
User Defined Displays the tool at a position defined by the user.
Note: You can define the tool position using Select a Tool from Session .
Tools
Only End Mill tools are available for thses operations.

Geometry

The Geometry tab allows you to define the geometric parameters that are machined.

Mandatory Parameters
Mandatory Parameter Description
Part Selects the part to machine.
Tool Axis Defines the tool axis.
Check Specifies surfaces to exlude from the machining activity (geometry saves on the deburring feature).

Strategy Parameters

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

Machining
Parameter Description
Guide Selects guide.
Start Direction Selects start direction.
Start Defines the start point.
End Defines the end point.
Tool Path Style Defines the tool path style duting machining.

Zig-zag The tool path alternates directions during successive passes.
One-way Next The tool path always has the same direction during successive passes. The tool goes diagonally from the end of one tool path to the beginning of the next.
One-way Same The tool path always has the same direction during successive passes. The tools returns to the first point in each pass before moving on to the first point in the next pass.

Machining Tolerance Specifies the maximum allowed distance between the theoretical and computed tool path.
Max Discretization Step Ensures linearity between points that are far apart.
Radial Strategy Parameters
Parameter Description
Stepover Side

Specifies how the distance between two consecutive paths is computed:

  • Left
  • Right

Distance on Guide Defines the distance between passes, on the guide.
Active Maximum Plunge Distance Prevents unwanted machining paths.
Lead Angle Defines the lead angle in the direction of motion.
High Speed Milling (HSM) Strategy Parameters
Parameter Description
High Speed Milling Specifies whether or not cornering for HSM is to be done on the trajectory.
Corner Radius Specifies the radius used for rounding the corners along the trajectory of an HSM operation. Value must be smaller than the tooltip radius.

Tool Axis Parameters

The Tool Axis tab allows you to define the too axis parameters that are machined.

Collisions Checking
The tab enables you to avoid collisions during machining.
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.
Check from Part Operation Considers Check defined in Part Operations.
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.
Machine Kinematics
This tab lets you correct problems encountered with respect of the machine kinematics.
Parameter Description
Optimize Machine Rotary Axis If selected, minimizes the variations of rotary degree of freedom, as well as tool axis variations.
Correct Out of Limit Points When this check box is selected, the points out of limits are removed:
  • If the point is out of limits in the X, Y, or Z-Axis, it is removed.
  • If the point is out of limits in the A, B, or C-axis, the tool axis is corrected and locked in the position limit.
  • If the point with the corrected axis is in collision, the point is removed.
Correct Large Angular Variation on Machine Rotary Axis If, between two points of the tool path, the variation on a rotary DOF (angular join of the machine) exceeds the Maximum variation, you can select one or several check boxes to modify the machine configuration. When you select several check boxes, the most appropriate one is applied to any given point.
  • Linking macro: The modification is done within the existing linking macro of the tool path.
  • Tool pass: When the tool is in contact with the part, you can define a Fanning Distance.
    Note: Entering 0mm deactivates the Fanning Distance.
  • Retract macro: A retract pass is added to reconfigure the machine.
Notes:
  • If problems subsist after computing the tool path with those options, a message is displayed.
  • These corrections apply to the tool path of the current machining operation.
  • The machine configuration on the first point of the current machining operation is seen as the result of a motion from the Home position to this first point. Thus, it may differ from the actual one, resulting from previous machining operation and machine instructions.
  • Angular variations between two points cannot be detected on the first point of the tool path, because the position of the machine before this point is unknown.

Macros Parameters

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

  • Approach
  • Retract
  • Clearance
  • Linking Retract
  • Linking Approach
  • Between Passes
  • Between Passes Link

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

Feeds and Speeds Parameters

The Feeds and Speeds tab allows you to define the following feeds and speeds parameters.

Feedrate
Parameter Description
Feedrate Unit Two available feedrate units:
  • Linear
  • Angular
Approach Feedrate Defines the speed of linear/angular advancement of the tool during its approach, before cutting.
Machining Feedrate Defines the speed of linear/angular advancement of the tool during machining.
Retract Feedrate Defines the speed of linear/angular advancement of the tool during its retract, after cutting.
Transition Activates the transition.
Feedrate Transition Transition options:
  • Machining
  • Approach
  • Retract
  • RAPID
  • Local
Local Value Specifies the local feedrate value.
RTCP ON When selected, activates RTCP mode on transition paths between the previous and current operations.
Spindle Speed
Parameter Description
Spindle Unit Angular or linear.
Machining Spindle Defines the speed of the spindle linear/angular advancement.