Multi-Axis Curve Machining

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

This dialog box contains controls for:

This page discusses:

See Also
Multi-Axis Curve Machining

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
End Mill tools , Conical tools , Lens Mill tools , Face Mill tools and TSlotter tools are available for these operations.

Geometry

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

Main Parameters
Parameter Description
Curve Machining Mode Specifies the curve machining mode.

Contact on Surface The tool follows the trajectory defined by the projection of the guiding contour on the part surface while respecting user-defined geometry limitations and machining strategy parameters.
Between Two Curves The tool follows a trajectory defined by the guide contour and auxiliary guide contour while respecting user-defined geometry limitations and machining strategy parameters.
Between Curve and Surfaces The tool follows trajectory defined by a top guide curve and bottom surfaces while respecting user-defined geometry limitations and machining strategy parameters.

Mandatory Parameters
Mandatory Parameter Description
Guides Selects the guides to machine.
Tool Axis Defines the tool axis.
Optional Parameters
Optional Parameter Description
Auxiliary Guides Positions the tool tip along the tool axis (axial positioning).
Start Defines the start point.
Stop Defines the end point.
Check Specifies surfaces to exlude from the machining activity (geometry saves on the deburring feature).
Other Parameters
Parameter Description
Offset on Contour Specifies the offset on contour.
Curve Machining Type Specifies the curve machining type. You can select one of the following types:
  • Side
  • Tip
Limits Specifies the limits.
Offset on Limits Specifies the offset on limits.

Strategy Parameters

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

Machining
Parameter Description
Tool Path Style Defines the tool path style during machining.

Zig-zag The tool path alternates directions during successive passes.
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.
Direction of Cut Specifies the cutting direction.

Climb The front of the tool (advancing in the machining direction) cuts into the material first.
Conventional The back of the tool (advancing in the machining direction) cuts into the material first.

Sequencing Defines the first axe to machined. You can select Radial First or Axial First.
Maximum Discretization Step Ensures linearity between points that are far apart.
Maximum Discretization Angle Specifies the maximum angular change of tool axis between tool positions.
Type of Contour Specifies the type of contour.

Circular The tool pivots around the corner point, following a contour whose radius is equal to the tool radius.
Angular The tool does not remain in contact with the corner point, following a contour comprised of two line segments.

Forced Contour Specifies whether the contour is to be forced open or closed.
Closed Contour Overlap Specifies the percentage of overlap on the closed contour.
Radial Parameters
Parameter Description
Distance Between Paths Defines the maximum distance between two consecutive tool paths in a radial strategy.
Number of Paths Defines the number of tool paths when the Number of Pathsstepover strategy is defined.
Axial Parameters
Parameter Description
Maximum Cut Depth Specifies the maximum cut depth the tool can realize during machining.
Number of Levels Specifies the number of levels to be machined.
Finishing Parameters
Parameter Description
Side Finish Pass Mode Specifies the side finish pass mode. You can select one of the following modes:
  • No Finish Pass
  • Side Finish at Last Level
  • Side Finish at Each Level
  • Finish Bottom Only
  • Side Finish at Each Level and Bottom
  • Side Finish at Last Level and Bottom
Side Finish Thickness Specifies the thickness of material that will be machined by the side finish pass.
Side FinishThickness on Bottom Specifies the thickness of material left on the side by the bottom finish pass.
Spring Path Indicates whether or not a spring pass is to be generated on the sides in the same condition as the previous side finish pass.
Bottom Finish Path Style Specifies the bottom finish path style: Zig-Zag or One-Way.
Tool Axis Strategy Parameters
Important:
  • Modifications of the tool axis generated by the mode you have selected apply only to the machining passes, not to the between paths passes.
  • For better performance and quality of the tool path, we recommend that you choose a tool axis as close as possible to the normal of the surface to be machined.
Parameter Description
Tool Axis Mode

Fixed Axis The tool axis arrow proposes a context menu:
  • Select: Defines the tool axis.
  • Analyze: Starts the Geometry Analyzer.
Interpolation The tool axis is interpolated between two selected axes.
Lead and Tilt The tool axis is normal to the part surface with respect to a given lead angle (alpha) in the forward tool motion and with respect to a given tilt angle (beta) in the perpendicular direction to this forward motion.
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.
Normal to Line The tool axis passes through a specified curve, and is normal to this curve at all points.
4 Axis Lead/Lag The tool axis is normal to the part surface with respect to a given lead angle in the forward direction and constrained to a specified plane.
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.

Tool Axis Parameters

Collisions Checking
Parameter Description
Activate collisions checking Activates or deactivates collisions checking.
Collision checking strategy Defines the strategy: Automatic or Removes Motions on Collisions.
Part, Check Enables collision checking on one or multiple elements.
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.
Maximum Angle Defines the maximum angle range within which the tool axis can vary.
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
  • Return in a Level Retract
  • Return in a Level Approach
  • Return Finish Pass Retract
  • Return Finish Pass Approach
  • Return Between Levels Retract
  • Return Between Levels Approach

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.
Finishing Feedrate Defines the speed of linear/angular advancement of the tool during finishing.
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.