Stiffener

The Stiffener dialog box appears when you select Stiffener from the Surface Machining section.

This dialog box contains controls for:

This page discusses:

See Also
Machining Stiffeners

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
End Mill tools and Conical tools are available for these operation.

Geometry

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

Mandatory Parameters
Parameter Description
Part Selects the part to machine.
Drive Specifies elements i.e. the stiffeners. They can be selected using the Face Wizard.
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).
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.
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.
  • Use the context menu item Offset to create a new safety plane, along the normal of the original safety plane, with the given offset value.
  • If the safety plane normal and the tool axis have opposed directions, the direction of the safety plane normal is inverted to ensure that the safety plane is not inside the part to machine.

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.
Lead angle Defines the lead angle of the tool axis.
Note: Lead angle is only available for the horizontal part of the stiffener.
Radial Strategy Parameters
Parameter Description
Activate radial steps When selected, the tool path includes radial steps.

By default, this check box is not selected.
Max. distance between pass Defines the depth of cut between two parallel passes.
Axial
Parameter Description
Number of Levels Specifies the number of levels to be machined.
Maximul cut depth Specifies the maximum cut depth the tool can realize during machining.

Tools Axis Parameters

The Tool Axis tab allows you to specify the following parameters.

Note: Those parameters are available only for NC Milling Machining built with Machine Tool Builder.
Tool Axis Parameters
Parameter Description
Optimize Machine Rotary Axis Optimizes the machine rotary axis.
Correct Out of Limit Points Corrects tool axis out of limit points.
Correct Large Angular Variation on Machine Rotary Axis Corrects large angular variation on machine rotary axis.

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

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.
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.