Multi-Axis Spiral Milling

  The information in this section will help you create and edit Multi-Axis Spiral Milling operations in your Machining program.

Click , then select the geometry to be machined. 

A number of strategy parameters are available.

Specify the tool to be used , feeds and speeds , and NC macros as needed.

Multi-Axis Spiral Milling: Strategy Parameters

The Multi-Axis Spiral Milling strategy parameters are distributed into 5 tabs:

In addition to the parameters available in those tabs, you have to select a tool path style, and to define the view axis, the tool axis and the start direction, depending on the tool path selected.

Tool path style

Indicates the cutting style of the operation:

  • Helical:
    the tool moves 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: this cutting style is made of two kinds of passes:
    • back and forth passes,
    • part contouring passes.
  • Contour only: only machines around the external contour of the part.
The tool path style is computed in 2D and then projected on the part surface. The distance between the resulting passes is modified according to the curve of the surface.
 

Tool Axis, View Direction, Start Direction

The tool axis is optional and used for Fixed axis strategy.
Place the cursor on the arrow A and right-click to display the contextual menu.

The item Select opens a dialog box to select the tool axis:

The view direction is visualized as the V axis.
Place the cursor on the arrow V and right-click to display the contextual menu.

The item Select opens a dialog box to select the view direction:

The Start direction is available for the Back and forth tool path style.
Place the cursor on the lower horizontal arrow S and right-click to display the contextual menu.

The item Select opens a dialog box to select the start direction:
 


You can choose between selection by Coordinates (X, Y, Z) or by Angles.
Angles lets you choose the machining direction by rotation around a main axis.
Angle 1 and Angle 2 are used to define the location of the machining direction around the main axis that you select.

Drop-down list

  • Feature-defined: you select a 3D element such as a plane that will serve to automatically define the best direction or axis.
  • Selection: you select a 2D element such as a line or a straight edge that will serve to define the direction or axis.
  • Manual: you enter the coordinates of the direction or axis.
  • Points in the view: click two points anywhere in the view to define the direction or axis.

sets the direction to that of the normal to screen.

The Reverse Direction button lets you reverse the direction of the axis with respect to the coordinate system origin.

The item Analyze opens the Geometry Analyser.

Multi-Axis Spiral Milling: Machining Parameters


Machining tolerance
Maximum allowed distance between the theoretical and computed tool path.
Consider the value to be the acceptable chord error.

Direction of cut
Specifies the position of the tool regarding the surface to be machined. It can be: 

Climb  or Conventional.
The cutting mode (Climb/Conventional) is respected on the contouring tool passes generated by the Helical tool path style.

Examples:

  • Direction of cut: Climb
    Tool path style: Helical
    Helical movement: Inward

    The contouring tool path is in blue,
    the roughing tool path is in green.
  • Direction of cut: Climb
    Tool path style: Helical
    Helical movement: Inward

    The contouring tool path is in blue,
    the roughing tool path is in green.

Helical movement
Available when Tool path style is set to Helical.

  • Outward: the tool path will begin at the middle of the area to machine and work outwards.
  • Inward: the tool path will begin at the outer limit of the area to machine and work inwards.

Max discretization angle
Specifies the maximum angular change of tool axis between tool positions.
It is used to add more tool positions (points and axis) if value is exceeded.

Always stay on bottom
Available when Tool path style is set to Helical or Back and forth.
When machining a multi-domain pocket using a helical tool path style, this parameter forces the tool to remain in contact with the pocket bottom when moving from one domain to another. This avoids unnecessary linking transitions.
Example:
Always stay on bottom is not active:

Always stay on bottom is active:

Multi-Axis Spiral Milling: Radial Parameters

Distance between paths
Specifies the distance between two consecutive paths.

Contouring pass
Available when the tool path style is set to Back and forth.
When selected, adds a contouring pass at the end of the back and forth path.

Multi-Axis Spiral Milling: Axial Parameters

Maximum cut depth
Depth of the cut effected by the tool at each pass.

Number of levels
Defines the number of parallel passes to be computed.

Multi-Axis Spiral Milling: Tool Axis Parameters

Note that modifications of the tool axis generated by the mode you have selected apply only to the machining passes, not to the between paths passes.

You can define several axes with this icon:

  • V, for the view direction,
  • A, for the tool axis direction.

The view directions defines the machining guiding plane: machining is done in planes parallel to the guiding plane.

The view direction defines the accessible areas for the tool. These areas are accessible if the angle between the view direction and the normal to surface is less than 85 degrees.

The tool axis definition depends on the Tool axis mode. The tool axis arrow turns white when its definition box is not available
(e.g. when the tool axis is defined through a point or a line, ...).

Clicking one of the direction arrows displays its definition box.

  • View direction:
  • Tool axis direction:

Tool axis mode
Note that modifications of the tool axis generated by the mode you have selected apply only to the machining passes, not to the between paths passes.


The tool axis can be fixed (see Tool Axis above) or normal to the part (i.e. the tool is normal to the bottom of the pocket with an angular tolerance).
When the tool axis is normal to the part, there is a risk of collision as shown below.
When the Tool axis mode is set to Normal to part, you must select the option Store contact points in tool path in the Tools > Options > Machining > Output tab in order to compute the tool path.
 

Multi-Axis Spiral Milling: HSM Parameters


Select the High Speed Milling check box to activate this mode.
The two tabs below becomes available. One deals with the corner tool passes, the other with the transition tool passes.

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. This ensures that there is no leftover material in the corners of the tool path.

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.

Multi-Axis Spiral Milling: Geometry

You can select:

  • a part to machine (mandatory) with a possible offset,
  • The thickness of the offset can be negative.
  • If you want to use a negative value, the tool corner radius must be greater than the absolute value of the offset.
 
  • guide faces (optional if soft guide contours are selected, mandatory otherwise) with possible offset. Guide faces:
    • can be used to define islands,
    • are used to compute the last pass in bitangency with the selected part.
In order to compute the bitangency, the tool radius must be higher than the corner formed by the part and the guide faces.
To get a regular tool path and tool axis variation, and a precise tool location on the path in bitangency, we recommend that you select all the guide faces where the tool can be in contact (i.e. the strip of vertical faces and the horizontal surfaces connex to the vertical ones) as shown below:
 
 
  • a soft guide contour (mandatory if guide faces are not selected, optional otherwise). It closes the guide faces if the pocket is open.
If the Tool axis mode is set to Normal to part:
  • a local reduction of the distance between paths can be observed near the soft guide because the tool contact point (and not the tool end point) is on the soft guide.
  • The Tool axis mode Normal to part is respected for Soft guide contours laying inside the Part surfaces; it may be not respected if Soft guide contours are laying on the Part surfaces boundary. In this case, the tool axis is computed with the help of the View Direction.
 
  • a check (optional) with possible offset,
Note that infinite geometries e.g. planes, selected as part or check geometries, are ignored in the tool path replay.
  • Start points: By default, there is no user-defined start point and the system determines automatically the start point.
    When several points are selected, the system automatically performs the mapping of each selected point with the area to be machined. In each area: 
    • when a point selected by the user exists, the system uses this point as start point,
    • when more than one point selected by the user exist, the system uses one of the user point (any of the selected ones).
    • the ordering of the selected points does not matter.
 
  • an offset group.

Geometry can also be defined using geometrical zones.

Collision Checking

Collision checking can be performed on the shank of the tool or on the shank of the tool plus the tool assembly (With tool assembly selected).
To save computation time, use tool assembly only if the geometry to be checked can interfere with the upper part of the cutter. 
You can define an Offset on tool and an Offset on tool assembly to avoid collisions.

Multi-Axis Spiral Milling: Tools

Recommended tools are end mill tools.

Multi-Axis Spiral Milling: Macro Parameters

General information about macros can be found in NC Macros.
Information about the operating mode can be found in Defining Macros.
Information about Surface Machining macro parameters can be found in Macro Parameters.

Standard macros are available:

  • approach macro to approach the operation start point,
  • retract macro to retract from the operation end points,
  • linking macros to link two non consecutive tool paths,
  • clearance macros.

The macros available for approach, retract and linking are:

Those for the clearance are: