Deburring Parameters

The Resource tab allows you to select a tool.

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 .

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

Mandatory Parameter	Description
Part	Selects the part to machine. Option Description Sharp Angle Filter Selects the sharp edges that have an opening angle lower than the defined maximum sharp angle. Limiting Plane Filter Selects the sharp edges located above the selected plane. Inclined Edges Filter Selects the sharp edges with a slope angle between the minimum and the maximum slope angles. Circular Edges Filter Selects the sharp edges that belong to holes with a greater diameter than the minimum radius. Machined Edges Filter Selects the previously machined sharp edges.
Sharp Edges	Selects the sharp edges to machine.

Optional Parameter	Description
Forbidden Edges	Specifies edges that must not be machined (geometry saves on the deburring feature).
Checks	Specifies surfaces to exlude from the machining activity (geometry saves on the deburring feature).
Safety Plane	It is the plane that the tool rises at the end of the tool path to avoid collisions with the part.

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

Table 1. Machining

Parameter	Description
Machining Tolerance	Specifies the maximum allowed distance between the theoretical and computed tool path.
Max Discretization Step	Ensures linearity between points that are far apart.
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.
Breakthrough	Specifies the distance in the tool axis direction that the tool must go completely through the part.
Mode	Specifies the sinking mode of the tool in the material.
Depth	Specifies the depth length of the tool sinking.
Compensation	Specifies the tool compensation site.

Table 2. Axial

Parameter	Description
Max Lead and Tilt Angle	Specifies a maximum lead angle and a user-defined inclination of the tool axis in a plane normal to the direction of motion. The tilt angle is with respect to the part surface normal.
Max Discretization Angle	Specifies the maximum angular change of tool axis between tool positions. It is used to add more tool positions (points and axis) if value is exceeded.

The Tool Axis tab allows you to select a new tool axis mode and perform a collision checking.

Table 3. Tool Axis Mode

Parameter	Description
No 3/5 Axis Converter	Forbids the computation of the tool path to convert a 3-axis machining operation into a 5-axis one.
Fixed Axis	The tool axis remains constant for the operation.
Thru a Point	The tool axis passes through a specified point. The tool axis can be oriented To the point or From the point.
Thru a Guide	The tool orientation is controlled by a geometric curve (guide), that must be continuous.
Fixed Angle	The tool axis forms an angle with the initial tool axis.
Normal to Drive Surface	Only the adjacent edges (among the selected edges) of the selected drive surfaces are machined. The tool axis is normal to the selected drive surfaces.
4 Axis	The tool axis is normal to the part surface with respect to a given lead angle in the forward direction and constrained to a specified plane.
Rolling	The tool axis is perpendicular to the average normal of the sharp edge.
Normal to Edge	The tool axis is aligned with the average normal of the sharp edge.

Table 4. Collision Checking

Parameter	Description
Activate Collisions Checking	Activates the collision checking when selected
Collision Checking Strategy	The two following modes are available: Remove Motions in Collisions and Automatic.
Part	Performs the collision checking on the part when checked.
Check	Performs the collision checking on the check when selected.
Design Part (PO)	Performs the collision checking on the design part of the part operation when selected.
Offset on Tool	Defines the offset applied on the tool to avoid collisions.
Offset on Tool Assembly	Defines the offset applied on the tool assembly to avoid collisions.
Max Discretization Angle	Specifies the maximum angular change of tool axis between tool positions. It is used to add more tool positions (points and axis) if the value is exceeded.
Minimum Length	Specifies the minimum distance that must exist between two collisions points to allow the modification of the tool axis between those two points.
Contact Point Position Range	Specifies the range of the contact points. It is defined as a ratio of the barrel arc length, centered on the initial contact point position.
Angle Mode	Specifies the tool axis mode: Lead or Tilt.
Minimum Angle	Defines the range within which the tool axis can vary.
Maximum Angle	Defines the range within which the tool axis can vary.
Step Angle	Defines the computation step used to find the optimal angle to avoid collisions.

The Macros tab allows you to define transition paths in your machining operations by means of NC macros.

The Feeds and Speeds tab allows you to define the following feeds and speeds parameters.

Table 5. 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 finish machining.
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.

Table 6. Spindle Speed

Parameter	Description
Spindle Unit	Angular or linear.
Spindle Output	Acivates/deactivates the NC output of the spindle speed.
Machining Spindle	Defines the speed of the spindle linear/angular advancement.