Multi-Axis Curve Machining: Between curve and part

This task shows how to insert a 'Between curve and part' Multi-Axis Curve Machining operation in the program.

To create the operation you must define:

the Curve Machining mode as Between curve and part and the Curve Machining type to Side
the geometry to be machined
the tool that will be used
the parameters of the machining strategy with the tool axis guided in Interpolation mode
the feedrates and spindle speeds
the macros (transition paths) .

Multi-Edition

You can modify the parameters of two or more Multi-Axis Curve Machining operations in one shot by means of the Selected Objects > Definition... contextual command.
See Editing Parameters of Several Multi-Axis Curve Machining Operations.

Open the MultiAxisMilling01.CATPart document, then select Machining > Advanced Machining from the Start menu.
Make the Manufacturing Program current in the specification tree.

Select the Multi-Axis Curve Machining icon .
The Multi-Axis Curve Machining dialog box appears directly at the Geometry tab page .
This page includes a sensitive icon to help you specify the geometry to be machined.
Set the Curve machining mode to Between curve and part.

The top guiding curve and part bottom in the icon are colored red indicating
that this geometry is required for defining the operation.
All other geometry is optional.

Set the Curve Machining type to Side to drive the tool flank.

Click the red bottom in the icon, then select the 6 faces in the 3D window as shown in the figure.
Click the top guiding curve in the icon, then select the 6 edges in the 3D window as shown in the figure.
The part and guide elements of the icon are now colored green indicating that this geometry is now defined.
These are also indicated on the part.

Select the Strategy tab page . You can then use the tab pages to set parameters for:

Machining

Radial (set Radial strategy with Distance between paths = 3mm and Number of paths = 4)

Axial

Finishing

Tool Axis (set to Interpolation).

Click the tool axis arrow (A) in the sensitive icon,
then specify the reference tool axis direction for the operation.
You can do this by selecting a surface. In this case the surface normal is used.
Click one of the red interpolation axes in the sensitive icon, then select a position for the first interpolation axis.
The axis is visualized by means of an arrow (I.1).
You can then specify the orientation of this axis using the Interpolation Axis dialog box that appears.
If you select a surface, the surface normal is used.
Select one or more positions for other interpolation axes and specify their orientations in the same way.

A tool is proposed by default when you want to create a machining operation.
If the proposed tool is not suitable, just select the Tool tab page

to specify the tool you want to use.
This is described in Edit the Tool of an Operation.

Select the Feeds and Speeds tab page to specify the feedrates and spindle speeds for the operation.
Check the validity of the operation by replaying the tool path.

You can add approach and retract motions to the operation in the Macros tab page

.
This is described in Define Macros of an Operation.

Click OK to create the operation.