Multi-Pockets Flank Contouring

The Multi-Pockets Flank Contouring dialog box appears when you select Multi-Pockets 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
Only End Mill tools and TSlotter tools are available for these operations.

Geometry

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

Mandatory Parameters
Mandatory Parameter Description
Part Selects the parts to machine.
Drive Defines the drive surfaces to be followed by the flank of the tool.
Tool Axis Defines the tool axis.
Optional Parameters
Optional Parameter Description
Check Specifies surfaces to exlude from the machining activity (geometry saves on the deburring feature).
Part Bottom Defines the bottom of the pocket.
Limiting Contour Defines the outer machining limit on the part. You can also activate the Part autolimit option, with the Side to machine, Stop position, Stop mode and Offset parameters.
Start Points Defines the start point.
Imposed Defines the imposed point.
Pocket Zone Order
Top Defines the highest plane machined on the part.
Bottom Defines the lowest plane machined on the part.
Safety Plane It is the plane that the tool rises at the end of the tool path to avoid collisions with the part.

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 Angle Specifies the maximum angular change of tool axis between tool positions.
Notes:
  • The Maximum discretization angle influences the number of points on the tool path: Choose its value carefully to avoid a high concentration of points along the tool trajectory.
  • Maximum discretization angle also applies to macro paths defined in machining feedrate. It does not apply to macro paths that do not have machining feedrate (RAPID, Approach, Retract, User, and so on).
Machining Tolerance Specifies the maximum allowed distance between the theoretical and computed tool path.
Cutting Mode Specifies the position of the tool regarding the surface to be machined.

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.
Either Either of the two possibilities may be used depending on which is most suitable to the current cutting action.

Machining Mode Specifies the machining mode.

By Plane The whole part is machined plane by plane.
By Area The whole part is machined area by area.

On Specifies the side of the part to machined.

Pockets Only Only pockets on the part are machined.
Outer Part Only the outside of the part is machined.
Outer Part and Pockets The whole part is machined outer area by outer area and then pocket by pocket.

Pass Overlap Defines an overlap distance of the end of a pass over the beginning.
Switch to Rapid Feedrate Defines the length of pass over which the feedrate value in the linking passes switches to a rapid one.
Stepover Parameters
Parameter Description
Sequencing Defines the first axe to machined. You can select Radial First or Axial First.
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.
Maximum Cut Depth Specifies the maximum cut depth the tool can realize during machining.
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
Side Finish Thickness Specifies the thickness of material that will be machined by the side finish pass.
Side Thickness on Bottom Finish Specifies the thickness of material left on the side by the bottom finish pass.
Axial Finish Distance Between Pass Specifies the maximum distance between two consecutive tool paths in an axial strategy.
Spring Path Indicates whether or not a spring pass is to be generated on the sides in the same condition as the previous side finish pass.
Tool Axis Strategy Parameters
Parameter Description
Guidance

Automatic Tilt The tool axis is tangent to the drive and is contained in a plane normal to the forward direction.
Along Isoparametrics The tool axis is tangent to the drive and follows the isoparametrics of the drive.

Fanning Distance Distance at the beginning and at the end of the motion where the fanning takes place.
Maximum Tilt Angle Maximum rotation angle of the tool around the contact point making the tool tangent to the drives.
High Speed Milling (HSM) Strategy Parameters
Parameter Description
Cornering Tool Path Specifies whether or not cornering for HSM is to be done on the trajectory.
Corner Radius Specifies the radius used to round the ends of passes to give a smoother path that is machined much faster.
Finishing Cornering Tool Path Activates finishing cornering tool path option.
Output Parameters
Parameter Description
Circular Interpolation Activates the arc interpolation output, when possible:
  • When the tool is in contact with a revolution surface with its axis parallel to the tool axis,
  • In the cornerization circular path,
  • And in circular motions of the macro.
Approximate Passes to Optimize Circular Interpolation Approximates the tool passes to optimize a circular interpolation when Circular Interpolation cannot be activated.
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
  • 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.
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.
Spindle Speed
Parameter Description
Spindle Unit Angular or linear.
Machining Spindle Defines the speed of the spindle linear/angular advancement.