Multi-Axis Swarf Milling

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

Note: Multi-Axis Swarf Milling behaves like Multi-Axis Flank Contouring operation. To create a Multi-Axis Swarf Milling operation, see Creating Multi-Axis Flank Contouring Operations

This dialog box contains controls for:

This page discusses:

See Also
Multi-Axis Swarf Milling

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 Swarf Milling operation are End Mills and T-Slotters .

Geometry

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

Mandatory Parameters
Parameter Description
Drive Defines the drive surfaces to be followed by the flank of the tool.
Start Element Defines the first drive on which the tool path starts.
Stop Element Defines the last drive on which the tool path ends.
Tool Axis Defines the tool axis.
Optional Parameters
Parameter Description
Part Selects the parts to machine.
Check Specifies surfaces to exlude from the machining activity (geometry saves on the deburring feature).
Other Parameters
Parameter Description
Start Positions the tool with respect to the start elements by selecting one of the proposed options:
  • In
  • On
  • Out
Stop Positions the tool with respect to the stop elements by selecting one of the proposed options:
  • In
  • On
  • Out
Offset Along Tool Axis Specifies the offset along the tool axis.

Strategy Parameters

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

Machining
Parameter Description
Machining Tolerance Specifies the maximum allowed distance between the theoretical and computed tool path.
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.
Close Tool Path Close strategy applied on the toolpath if the drive is closed.The first and the last point of the pass are then the same.
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.

Sequencing Defines the first axe to machined. You can select Radial First or Axial First.
Radial Strategy Defines the radial strategy.
Distance Between Paths Defines the maximum distance between two consecutive tool paths in a radial strategy.
Number of Paths Defines the number of radial pass.
Axial Strategy
Mode Specifies the axial mode. You can select one of the following modes:
  • Interpolate
  • Constant
Distance Between Paths Defines the maximum distance between two consecutive tool paths in an axial strategy.
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
Tool Axis Strategy Parameters
Parameter Description
Fixed Axis for Semi-Finishing Paths Defines useful cutting length on current tool when Control Fanning Using Tool Parameter is activated.
Guidance Specifies the tool axis strategy.

Tanto Fan The tool is tangent to the drive surface at a given contact height, and the tool axis is interpolated between the start and end positions.
Fixed Axis The orientation of the tool axis is fixed.

Contact Height Determines a point on the drive surface where the tool must respect tangency conditions. The Contact Height is measured from the tool tip along the tool axis. The point on the drive is computed such that its projection normal to the drive onto the tool axis respects the Contact Height value.
Tilt Angle Specifies a positive angle to lean the tool right.
Note: Tilt angle parameter is disabled in Fixed Axis mode.
Lead Angle Specifies a positive angle to lean the tool forwards.
Note: Lead Angle parameter is disabled in Fixed Axis mode. Sometimes with Tanto Fan mode, constraints on the tool path cannot be applied.
High Speed Milling (HSM) Strategy Parameters
Parameter Description
Cornering Specifies whether or not cornering is to be done on the trajectory for HSM.
Radius Specifies the radius used for rounding the corners along the trajectory of a HSM operation. Value must be smaller than the tool radius.
Finishing Cornering Specifies whether or not tool path cornering is to be done on side finish paths.
Radius Specifies the corner radius used for rounding the corners along the side finish path of a HSM operation. Value must be smaller than the tool radius.
Output Parameters
Parameter Description
Output Type Defines the output type:
  • No
  • 3d Radial (PQR)
  • 2D Radial - TIP (G41/G42)

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
  • 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.

Feed reduction is applied to corners along the tool path whose radius is less than the Maximum radius value and whose arc angle is greater than the Minimum angle value. Corners can be angled or rounded.

For Multi-Axis Flank Contouring, feedrate reduction applies to inside corners for machining or finishing passes. It does not apply to macros or default linking and return motions.

If a cornering is defined with a radius of 5mm and the Feedrate reduction in corners is set with a smaller radius value, the feedrate will not be reduced.

Feedrate Reduction in Corners Combined with Local Slowdown Rate
If the Feedrate reduction in corners option is selected and local Slowdown rates are applied to drives, the general rule is that the corner feedrate reduction rate is applied after the local Slowdown rate on the current feedrate. For a machining feedrate, the feedrate will be equal to:

machining feedrate * local Slowdown rate * corner Reduction rate.

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