Multi-Axis Spiral Milling

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

This page discusses:

See Also
Creating an Multi-Axis Spiral Milling 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
Recommended tools for Multi-Axis Spiral Milling are End Mill tools and Lens Mill tools .

Geometry

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

Mandatory Parameters
Parameter Description
Parts Selects the parts to machine.
Guides Selects the guides to machine.
Soft Guide Contour Defines the soft guide contour.
Tool Axis Defines the tool axis.
Optional Parameters
Parameter Description
Check Specifies surfaces to exlude from the machining activity (geometry saves on the deburring feature).
Start Points Defines the start point.

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 duting machining.

Helical Moves the tool in successive concentric passes from the boundary of the area to machine towards the interior. The tool moves from one pass to the next by stepping over.
Back and Forth Alternates tool-path motions between one direction and its opposite.
Contour Only Machines only around the external contour of the part.
Concentric Builds a safe-cutting trajectory by controlling the engagement of the tool. The created trajectory adapts itself dynamically to ensure a safe cutting at nominal speed.
Notes:
  • This strategy is recommended for hard-material milling.
  • In this type of material, the tool needs to be protected.

View Direction Defines the accessible areas for the tool
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 Angle Specifies the maximum angular change of tool axis between tool positions.
Always Stay on Bottom Forces the tool to remain in contact with the pocket bottom when moving from one domain to another. Available when machining a multi-domain pocket using a helical tool path style.
Radial Strategy Parameters
Parameter Description
Maximum Distance Between Paths Defines the maximum distance between two consecutive tool paths in a radial strategy.
Contouring Pass Adds a contouring pass at the end of the back and forth path.
Contouring Ratio Defines the contouring ratio.
Axial
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.
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.

High Speed Milling (HSM) Strategy Parameters
Parameter Description
High Speed Milling Cornering

Corner Radius Specifies the radius used to round the ends of passes to give a smoother path that is machined much faster.
Limit Angle Specifies the minimum angle the tool pass must form to allow the rounding of the corners.
Extra Segment Overlap Specifies an overlap for the extra segments that are generated for cornering in a high speed milling operation.
Transition Radius Specifies the radius at the extremities of a transition path in a high speed milling operation.
Transition Angle Specifies the angle of the transition path that ensures a smooth move from one path to another in a high speed milling operation.
Transition Length Specifies the minimum length of the straight segment of the transition path in a high speed milling operation.

Tool Axis Parameters

Collisions Checking
Parameter Description
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.
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.