Multi-Axis Curve Engraving

The Multi-Axis Curve Engraving dialog box provides options for defining a Multi-Axis Curve Engraving machining operation.

To access the dialog box, select Multi-Axis Curve Engraving

This page discusses:

Resource Parameters

The Resource tab allows you to select a tool.

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 .

Geometry

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

Mandatory Parameter Description
Parts Selects the parts to machine.
Guides Defines guide surfaces.
Optional Parameter Description
Start Defines a start point.
Stop Defines an end point.
Check Specifies surfaces to exlude from the machining activity (geometry saves on the deburring feature).
Engraving Depth Specifies the engraving depth.

Strategy Parameters

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

Table 1. Machining
Parameter Description
View Direction Defines the accessible areas for the tool
Engraving Mode Defines the tool path style duting machining.

Letters Creates geometry using Text in Sketcher or a set
Stripes Creates stripes in a set of curves.
Trimming Defines trimming as the engraving mode.

Orientation Set the Left or Right orientation.
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.

Helical Movement

Inward Starts the tool path at the outer limit of the area to machine and work inwards.
Outward Starts the tool path at the middle of the area to machine and work outwards.

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.
Forced Contour Specifies whether the contour is to be forced open or closed, or not. Applies to trimming.
Closed Contour Overlap Specifies the percentage of overlap on the closed contour. Applies to trimming.

Table 2. Tool Axis Strategy Parameters
Parameter Description
Tool Axis Mode

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.
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.
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.
Optimized Lead The tool axis is allowed to vary from the specified lead angle within an allowed range.
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 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.

Maximum Lead and Tilt Angle Maximum allowed angle that avoid collisions with the part.

Tool Axis Parameters

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.

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 Between 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.

Table 3. 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.
Table 4. Spindle Speed
Parameter Description
Spindle Unit Angular or linear.
Machining Spindle Defines the speed of the spindle linear/angular advancement.