Multi-Axis Sweeping 

  The information in this section will help you create and edit Multi-Axis Sweeping  operations in your Machining program.
Click , then select the geometry to be machined . 

More information can be found in Selecting Geometry.

A number of strategy parameters are available for defining:

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

The Stepover tab has been renamed into Radial tab.

Multi-Axis Sweeping: Strategy Parameters

Multi-Axis Sweeping: Machining Parameters

Tool path style
Indicates the cutting mode of the operation:

  • Zig Zag: the machining direction is reversed from one path to the next
  • 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.
Consider it to be the acceptable chord error.

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.
It is used to add more tool positions (points and axis) if value is exceeded.

Minimum path length
Specifies the minimum length of path to be taken into account.

  • The Maximum discretization step and Maximum discretization angle influence the number of points on the tool path.
  • The values should be chosen carefully if you want to avoid having a high concentration of points along the tool trajectory.
  • These parameters also apply to macro paths that are defined in machining feedrate.
    They do not apply to macro paths that do not have machining feedrate (RAPID, Approach, Retract, User, and so on).
  • Default value for Maximum discretization step is 100 m. Default value for Maximum discretization angle is 180 degrees.
 

Multi-Axis Sweeping: Radial Parameters

Radial strategy


Defines how the distance between two consecutive paths is to be computed.

Scallop height:


The associated parameter is Scallop height that specifies the maximum scallop height between
two consecutive tool paths in a radial strategy.
Note that the machining tolerance influences the distance between two consecutive paths.
When the machining tolerance value is increased, the distance between two consecutive paths is decreased according to the specified maximum scallop height value.

Distance on part:


The associated parameter is Distance between paths that defines the maximum distance between
two consecutive tool paths in a radial strategy.

Distance on plane:


The associated parameter is Distance between paths that defines the maximum distance between
two consecutive tool paths in a radial strategy.

Number of paths:


The associated parameter is Number of paths that defines the number of tool paths in a radial strategy.

Stepover side
Specifies the side of the guiding plane that will be used to determine the overall machining direction.

Multi-Axis Sweeping: Tool Axis Parameters

(Only Tool Axis Parameters tabs containing parameters have been captured)

You can define several axes with this icon:

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

The view and the start directions define the machining guiding plane: machining is done in planes parallel to the guiding plane.

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, ...).

A click one of the direction arrows displays its definition box.

  • View direction:
  • Start direction:
  • Tool axis direction:

Tool axis mode


Specifies how the tool axis is to be guided.

Below you will find the explanations of the various modes, then the explanations of the associated parameters.

Lead and Tilt

In this mode 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. 

There are several guidance modes as follows:

Fixed lead and tilt: 


Here both the lead and tilt angles are constant.

Variable lead and fixed tilt:


Here the tool axis can vary from the specified lead angle within an allowed range, the tilt angle remaining constant.
The allowed range is defined by Minimum and Maximum lead angles.

Fixed lead and variable tilt:


Here the tool axis can vary from the specified tilt angle within an allowed range, the lead angle remaining constant.
The allowed range is defined by an Allowed tilt (the tool axis can move within a range of +/ - Allowed tilt angle).
The purpose of the variable modes is to avoid collisions between the part to machine and the tool.
 

Fixed Axis


The tool axis remains constant for the operation.

Thru a Point

The tool axis passes through a specified point. The tool axis can be oriented To the point  or From the point.


Click the point in the sensitive icon and select a point in the graphic area.
Then decide whether the tool axis is defined from that point

or to that point

by clicking of the toggle From/To in the sensitive icon.

Normal to Line

The tool axis passes through a specified curve, and is normal to this curve at all points.
The tool axis can be oriented To the line or From the line.

Click the point in the sensitive icon and select a line in the graphic area.

Then decide whether the tool axis is defined from that line

or to that line

by clicking of the toggle From/To in the sensitive icon.

Optimized Lead

Optimized lead is not available for a barrel tool.

The tool axis is allowed to vary from the specified lead angle within an allowed range.
The allowed range is defined by Minimum and Maximum lead angles.
The back of the cutter is to be kept clear of the part by means of a Minimum heel distance.

Optimized lead works as follows:

  • lead defined as minimum to fit the part curvature
  • lead increases if necessary to respect the Minimum heel distance.

If the required lead is outside the allowed range, the tool position will not be kept in the tool path.
The maximum material removal is obtained when the tool curvature along the trajectory matches the part curvature.

C1= tool curvature along motion
C2= part curvature along motion

4-axis Lead/Lag

4-Axis lead/lag is not available for a barrel tool.

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. 

Click the 4-Axis Constraint arrow (N  in the 3D window or the arrow normal to the plane in the sensitive icon) and set this direction in the dialog box that appears. This is the normal to the plane in which the tool axis is constrained.

The tool axis is computed like in Lead and Tilt mode and then projected into the constraint plane.

Lead angle
Specifies a user-defined incline of the tool axis in a plane defined by the direction of motion and
the normal to the part surface.
The lead angle is with respect to the part surface normal.

Maximum lead angle
Specifies a maximum lead angle.

Minimum lead angle
Specifies a minimum lead angle.

Tilt angle
Specifies a user-defined incline of the tool axis in a plane normal to the direction of motion. 
The tilt angle is with respect to the part surface normal.

Allowed tilt
Specifies the range of allowed tilt variation.

Minimum heel distance

Allows the back of the cutter to be kept clear of the part
(for example, when machining a smooth concave ruled part in Optimized Lead).
 

Thru a guide

This strategy is used mainly to machine revolute surfaces, e.g. hub machining, deep pockets, ...
The tool orientation is controlled by a geometrical curve (guide), that must be continuous.
An open guide can be extrapolated at its extremities.
Click the red curve in the sensitive icon and select a curve in the 3D viewer.
The tool can be oriented From or To the guide.

Mode


Defines how the position of the tool is computed:

  • Normal to the path: for a given contact point, the intersection of the plane normal to the path with the guide give the tilt angle of tool.
    If several intersection are found, the nearest one is taken into account.
  • Nearest position: the tool is oriented by the point that gives the shortest distance between the guide and the contact point.
  • Nearest position along view direction: the guide is projected on a plane normal to the view direction.
    The tool is oriented by the point that give the shortest distance between the projected guide and the current contact point.

Offset on guide

You can define an offset on the guide. The offset is computed on a plane defined by the tangent of the guide and the view direction.
Click the Axis Guide arrow to define on which side the offset is applied.

Extend guide

Select this check box to extrapolate the extremities of an open guide.
 

Multi-Axis Sweeping: Cutter Compensation Parameters

(Double-click the part operation and push the Machine icon to open the Machine Editor)

In the Machine Editor, the Compensation tab contains options for:

  • globally defining the 3D contact cutter compensation mode: None/Contact/Tip and Contact
  • imposing the compensation mode to all operations supporting the selected mode
    whatever the choice defined at machining operation level.

If the options are set as follows, compensation can be managed at machining operation level.

In this case a Compensation tab appears in the Strategy page of the machining operation editor,
and the following options are available.

Output type
Allows you to manage the generation of Cutter compensation (CUTCOM) instructions in the NC data output:

The following options are proposed:

3D Contact (G29/CAT3Dxx)

The tool contact point will be visualized during tool path replay. 
Cutter compensation instructions are automatically generated in the NC data output.
An approach macro must be defined to allow the compensation to be applied.
Example of generated APT source:

$$ Start generation of : Multi-Axis Sweeping.1
FEDRAT/ 1000.0000,MMPM
SPINDL/ 70.0000,RPM,CLW
CUTCOM/NORMPS
$$ START CUTCOM NORMPS XC, YC, ZC, XN, YN, ZN, I, J, K
.../...
CUTCOM/OFF
$$ END CUTCOM NORMPS XC, YC, ZC, XN, YN, ZN, I, J, K
$$ End of generation of : Multi-Axis Sweeping.1

None

Cutter compensation instructions are not automatically generated in the NC data output.
However, CUTCOM instructions can be inserted manually.
For more information, please refer to How to generate CUTCOM syntaxes provided in the Prismatic Machining User's Guide. 

Multi-Axis Sweeping: Geometry

You can specify the following Geometry:

  • Part with possible Offset on Part. 
  • Check elements with possible Offset on Check.
  • Areas to avoid.
  • Limiting Contour with possible offset.

    The area to machine is defined by the projection of the limiting contour on the part along the view direction.
    The value of Offset can be positive, to extend the area to machine (up to the part boundaries),

    or negative to reduce the area to machine.

    The Limiting Contour re-limits the contact path (in red above) and not the tool tip path (in green above).
    Side to machine lets you define which portion of the part you want to machine (Inside or Outside of the limiting contour).

You can use Offset Groups and Features when defining geometry.
In R13, the behavior of offset group has changed and is now similar to that of 3 Axis Surface Machining.
 

Collision Checking is also available.

Multi-Axis Sweeping: Tools

Recommended tools for Multi-Axis Sweeping are End Mills, Face Mills, Conical Mills, T-Slotters and barrel tools.

In general, you should choose:

  • a ball-end tool for Fixed lead and variable tilt tool axis guidance
  • a filleted-end tool for Variable lead and fixed tilt tool axis guidance.
  • a barrel tool to machine composite structures, for the Fixed axis, Lead and tilt, Thru a point and Normal to line tool axis modes (4-Axis lead/lag and Optimized lead are not available for this tool).
 

Multi-Axis Sweeping: Feeds and Speeds

In the Feeds and Speeds tab page, feedrates for approach, retract and machining as well as a machining spindle speed.
Feedrates and spindle speed can be defined in linear or angular units.

A Spindle output checkbox is available for managing output of the SPINDL instruction in the generated NC data  file.
If the checkbox is selected, the instruction is generated. Otherwise, it is not generated. 

Feeds and speeds of the operation can be updated automatically according to tooling data and
the Rough or Finish quality of the operation.
This is described in Update of Feeds and Speeds on Machining Operation.

Multi-Axis Sweeping: NC Macros

You can define transition paths in your machining operations by means of NC Macros. 
These transition paths are useful for providing approach, retract, return, and linking motion in the tool path. 

  • An Approach macro is used to approach the operation start point.
  • A Retract macro is used to retract from the operation end point.

  • A Linking macro may be to link two non consecutive paths, for example. It comprises an approach and a retract path.

  • A Return in a Level macro is used in a multi-path operation to link two consecutive paths in a given level.
    It comprises an approach and a retract path.
  • A Clearance macro can be used in a machining operation to avoid a fixture, for example.