3D Finishing

Select Favorite

Instead of modifying n values, this option allows you to restore (or save) values that have already been entered.

Select the tool to use

By default, if the previous operation tool can be used, it is reused for this operation (the name of the tool appears in the graphic area next to )

If the previous tool is not suitable or if this is the first operation, you must select a tool to validate the operation ()

Define Cutting Conditions for Operation

Use this icon to modify the cutting conditions of the current operation.

Define or Add Geometries to Machine

Use this icon to select (or remove) machinable geometries.

This geometry is automatically added, by first selecting the geometry and right-clicking "End Milling". By doing this you won't need to access to this icon.

Define Milling Boundaries

You can also apply trims (XYZ or contour) to the current operation.

For a 3D finishing, bounding curves must be on the part.

Define all milling settings

Each milling has specific settings. Use this icon to access all settings (such as stocks to leave, altitudes, plunge modes, milling modes, etc.)

Define ISO File Settings

Use this icon to define which comment to use for the ISO code or to decide which inclined plane matrices to use.

Define colinear axis

This icon is available only if the current machine has colinear axis.With this icon it will then be possible to choose the axis drives by the operation.We also can choose the Z value of the fix axis.

Allow us to add one or more axis on the current machining

With this icon it is possible for example to make radial, axial or tilt the operation.

Define Operation Properties

Use this icon to define whether you would like to update the stock or calculate the result later.

Confirm

To confirm the current operation,

pressing this icon

to right-click outside the window and use the "OK" menu

Cancel

If you wish to cancel the operation, click this icon.

Preview

          Display or hide the machining area.

When this is hidden, this area is not calculated, and response times improve.

Show Label

           Allows you to display or hide the graphic area label.

Editing Update

Each time a setting is changed (such as the axial depth), all calculations for updating the hatching area and the trajectory are triggered.

The setting change may take a few moments.

In several cases, settings must be modified before updating the calculations. For this, press this icon. In the case, the hatching area and trajectory (for example) are not recalculated before pressing this icon again.

 Raster passes   

The parallel plane milling mode allows you to automate the creation of paths using the same principle as the old machines to be copied. The tool follows the digital shape to complete like a spindle follows a wood model, the movements of this spindle being locked on an axis such that it can only move perpendicularly along the XY plane.

Constant Pitch

Particularly for part finishing, this type of operation consists of automatically milling a part made up of a set of faces by completing a series of concentric contourings and varying the space between each face in order to maintain the height of the scallop no matter the curved surface of the part using a contour provided by the operator.

Two conditions must be respected for the tool path calculation:

• The scallop height must be less than twice the computing tolerance.

• The Step over must be lower than 1/3 of the radius. (what we call radius is the tool radius for a ball nose mill and the corner radius for a radiused mill).

If a gap is applied, the step over must be less than (tool radius - gap) / 3.

  Constant Z

This technique allows you to use the best cutting conditions for the greatest productivity. The cutting speed required is followed because the tool rarely mills to the center. In addition, the feed rate remains constant, and the tool only descends when the Z plane is changed.

Projection

The faces that make up the model to mill are cut into radial planes containing the segment defined by the user in the guide curve. These planes are regularly spaced at a radial pitch.

Milling is completed longitudinally in the direction of the revolution axis. The step over movement can be a square cycle or classic zigzag, staying in contact with the part or not.

Morphing

This technique allows you to mill a part to avoid jumps on the trajectory and "esthetic" marks on the part.

Spiral milling is then completed. To avoid rapid jumps, the scallop value is decreased to force the tool to redo the areas requiring rapid jumps.

You must select a starting curve, an ending curve (or a point), and their points of origin. These points must be aligned so that the pass spirals are best calculated.

You can optimize the trajectory so that it is more "fluid" by selecting intermediate curves.

Projected Spiral

This feature is specifically for semi-finishing parts. This type of operation consists of automatically milling a part made up of a set of faces by completing a series of concentric contourings projected onto the part.

The user resolves the main part geometry problems, such as:

• Minimum Curvature Radius

• Triangular Surfaces

• Overlapping Surfaces

• Undercut Surfaces

• Holes

Type of Machining

Computing Tolerance

0.02mm

Stock to leave on floor

0mm

Stock to leave on side

0mm

Step overs

0.5mm

Scallop Heights

0.0209mm

Sweeping Angle

0°

Machine visibility

WCS visibility

Tool visibility

Collision visibility

Stock and finish visibility

 Tool paths visibility

• Instead of entering all of the settings for each of these icons, you can also copy the settings that have already been entered into an operation by dragging this operation (with the left mouse button) from the operations list to the icon where you wish to copy.