Multi-Axis Flank Contouring

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

This dialog box contains controls for:

This page discusses:

See Also
Creating Multi-Axis Flank Contouring Operations

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 Flank Contouring operation are End Mills , Conical Mills , T-Slotters , and Barrel tools .

Geometry

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

Mandatory Parameters
Parameter Description
Part Selects the parts to machine.
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
Check Specifies surfaces to exlude from the machining activity (geometry saves on the deburring feature).
Refrence Point Defines a refrence point for the start position.
Auxiliary Guiding Curve Modifies the tool axis strategy to avoid collisions at the top of drive elements or to keep a safety distance on these elements.
4 Axis Plane Constraint - Optional 4 Axis Plane Defines the 4 axis plane constraint and/or the optional 4 axis plane
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

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 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.
Close Tool Path Specifies that the first drive is also used as the last drive.
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.
Maximum Distance Between Step Specifies the maximum distance between points. It is used to detect the end of drive elements.
Manual Direction Specifies the direction on the first drive. You can select one of the following directions:
  • Left
  • Right
  • Auto
Radial and Axial
Parameter Description
Distance Between Paths Defines the maximum distance between two consecutive tool paths in a radial strategy.
Number of Paths Defines the number of tool paths when the Number of Pathsstepover strategy is defined.
Mode Specifies the axial mode. You can select one of the following modes:
  • By Offset
  • By Thickness
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.
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
Control Fanning Using Tool Parameter Enables you to control tool fanning or the offset distance when approaching drive surfaces with negative draft angles, without needing to modify the tool chosen in the database.
Useful Cutting Length Defines usefull cutting length on current tool when Control Fanning Using Tool Parameter is activated.
Use of Guide Curve Tool can be made to respect the guide curve either Always or If Needed.
Tool Axis Strategy 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.
Combin Tanto This strategy combines three phases:
  • Tool fans over a given leave fanning distance.
  • Tool is tangent to the drive surface at a given contact height and is contained in a plane normal to forward direction.
  • Tool fans over a given approach fanning distance.
Combin Parelm This strategy combines three phases:
  • Tool fans over a given leave fanning distance.
  • Tool is tangent to the drive surface at a given contact height and follows the surface isoparametrics.
  • Tool fans over a given approach fanning distance.
Mixed Combin Either Combin Parelm or Combin Tanto is applied depending on the drive surface geometry. Combin Tanto is applied for cylindrical and planar drives. Combin Parelm is applied for other drive surface geometry.
Fixed Axis The orientation of the tool axis is fixed.
Normal to Part The tool axis remains normal to the part surface while the tool remains in contact with the drive surface.

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

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.
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.