Multi-Axis Curve Machining: Between 2 curves with Tangent Axis Guidance

task target This task shows how to insert a 'Between 2 curves' Multi-Axis Curve Machining operation in the program.

In this scenario the tool axis will be guided in Tangent Axis mode along the isoparametrics of the selected drive surfaces.

To create the operation you must define:

  • the Curve Machining mode as Between 2 curves and the Curve Machining type as Side
  • the tool that will be used

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.

pre-requisites Open the MultiAxisMilling03.CATPart document, then select Machining > Advanced Machining from the Start menu.
Make the Manufacturing Program current in the specification tree.  
scenario

  1. 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 2 curves.

  2. Click the top guiding curve in the icon.
    In the Edge Selection toolbar that appears, set Link types to Insert line
    then select the three edges on the part as shown in the figure below.
    Note that any gaps between the edges are filled thanks to the Insert link option.

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

  4. Select the Strategy tab page .
    This page includes a sensitive icon to help you specify the drive surfaces and reference tool axis.
    You can use the tab pages to set parameters for:

    • Tool Axis  (set to Tangent Axis - Along isoparametric lines).

  5. Click the sensitive drive element in the icon,
    then select the three drive surfaces in the 3D window as shown in the figure. 
 
A default reference tool axis is displayed in the 3D view.
If needed, you can modify it by clicking the tool axis arrow (A) in the sensitive icon, then specifying a different tool axis direction.
You can do this by selecting a surface. In this case the surface normal is used.

When machining a strip (or band) for faces, the tool axis is deduced from the isoparametrics of the faces
in order to ensure continuity of the trajectory. See Tangent Axis - Along isoparametric lines for more information.
 

  1. 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.

  2. Select the Feeds and Speeds tab page to specify the feedrates and spindle speeds for the operation.

  3. 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.

  1. Click OK to create the operation.

end of task