Multi-Axis Surface Engraving

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 operations.

Geometry

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

Mandatory Parameters

Mandatory Parameter	Description
Bottom(s)	Defines bottom surfaces.
Guides	Defines guide surfaces.

Optional Parameters

Parameter	Description
Check	Specifies surfaces to exlude from the machining activity (geometry saves on the deburring feature).
Start Point	Defines a start point.
Side for Offset	Defines the side On, Inside or Outside for the offset.
Engraving Depth	Defines the engraving depth.

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 duting machining. Helical Moves the tool in successive concentric passes from the boundary of the area to machine towards the interior. The tool moves from one pass to the next by stepping over. Back and Forth Alternates tool-path motions between one direction and its opposite. Contour Only Machines only around the external contour of the part. Concentric Builds a safe-cutting trajectory by controlling the engagement of the tool.
View Direction	Defines the accessible areas for the tool
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.
Helical Movement	Inward Starts the tool path at the outer limit of the area to machine and work inwards. Outward Starts the tool path at the middle of the area to machine and work outwards.
Maximum Discretization Angle	Specifies the maximum angular change of tool axis between tool positions.
Always Stay on Bottom	Forces the tool to remain in contact with the pocket bottom when moving from one domain to another. Available when machining a multi-domain pocket using a helical tool path style.

Radial Strategy Parameters

Parameter	Description
Radial Strategy	Defines the radial strategy as Tool Diameter Ratio or Maximum Distance.
Maximum Distance Between Paths	Defines the maximum distance between two consecutive tool paths in a radial strategy.
Percentage of Tool Diameter	Defines the percentage of the tool diameter.
Number of Contouring Pass	Defines the number of contouring paths.
Contouring Pass	Adds a contouring pass at the end of the back and forth path.
Contouring Ratio	Defines the contouring ratio.

High Speed Milling (HSM) Strategy Parameters

Parameter	Description
HSM Cornering	Activates the HSM cornering mode.
Corner Radius	Specifies the radius used for rounding the corners along the trajectory of an HSM operation. Value must be smaller than the tooltip radius.

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.

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.
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.