Impeller Hub Machining

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 , Conical tools and Lens Mill tools are available for these operations.

Geometry

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

Mandatory Parameters

Parameter	Description
Part	Selects the parts to machine.
First Blade	Defines a set of faces that represent the blade.
Top First Blade	Deffines a set of guide lines that represents the top of the blade.
Second Blade	Defines a set of guide line that represents the boundary between the hub and the blade.
Hub	Defines the hub to machine.
Revolution Axis	Defines the revolution axis.

Optional Parameters

Parameter	Description
Splitters	Defines a set of faces that represents the splitter.
Top Splitters	Defines a set of guide lines that represents the top of the splitter.
Bottom Splitters	Defines a set of guide lines that represents the bottom of the splitter.
Safety Plane	It is the plane that the tool rises at the end of the tool path to avoid collisions with the part.
Offset on Impeller	Defines an offset on impeller.
Radial Offset on Blades/Splitters	Defines the offset.

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.
Direction of Cut	Specifies the cutting direction. 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.
Stepover	Specifies how the distance between two consecutive paths is computed: Via scallop Height Constant
Scallop Height	Defines scallop height.
Radial Distance Between Paths	Defines the radial distance between paths.

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.

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.