Create a Multi-Axis Helix Machining Operation in Interpolation Mode

task target This task illustrates how to insert a Multi-Axis Helix Machining operation in the program. This operation will be used to generate a single helix toolpath to mill a blisk blade, while avoiding collisions with neighboring blades.

The scenario below show how to quickly create an operation. The recommended procedure is described in Collision-Free Multi-Axis Helix Machining in the Methodology section.

To create the operation you must define:

  • the tool that will be used
  • the parameters of the machining strategy with the tool axis guided in Interpolation mode
pre-requisites Open the Blisk.CATPart document, then select Machining > Advanced Machining from the Start menu. Make the Manufacturing Program current in the specification tree. 

The following procedure describes how to machine the middle (green) blade with no tool collisions with the two neighboring blades.
scenario 1. Select the Multi-Axis Helix Machining icon . A Helix Machining entity along with a default tool is added to the program. The Multi-Axis Helix Machining dialog box appears directly at the Geometry tab page .

The part surface, upper and lower contours, and leading and trailing edges of the sensitive icon are colored red indicating that this geometry is required and must be selected. The upper and lower contours and the leading and trailing edges must lie on the faces selected as part surface.

Selection of check elements (such as neighboring blades or fixtures) is optional.

2. Click the red part surface in the icon then select the faces to be machined in the 3D window. In this scenario, you must select 4 faces: the front face, the back face, the leading face, and the trailing face.

The Face Selection toolbar appears to help you select these faces. Note that faces must be continuous. Gaps between faces may result in a bad tool path.
3. Select the upper and lower contours. The Edge Selection toolbar appears to help you select these contours. They must be closed contours.
4. Select the leading and trailing edges to define the limits of the machining. The Edge Selection toolbar appears to help you select these edges. They must intersect the upper and lower contours.
   
  • The geometry entities of the icon are now colored green indicating that this geometry is now defined.
  • At this stage, make sure the Collision Checking option in the Geometry tab is deactivated.
  5. 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. For example, you can create a conical mill tool with the following characteristics.

Please refer to Edit the Tool of an Operation for more information.
6. Select the Strategy tab page .

Set the Tool axis mode to Interpolation.
Select a Start point by clicking on the sensitive icon then picking any point on the part surface.
  7. Click one of the interpolation axis symbols in the sensitive icon.

Default Interpolation axes (I.1 to I.4) are displayed at the four corners of the part.

The Interpolation Axes dialog box is displayed.

All the interpolation vectors are listed with their position, direction and status.
Pick a vector in the dialog box. It is highlighted in the 3D viewer.
Click to add an interpolation vector:
The Interpolation Axes dialog box disappears.
Pick in the 3D viewer to indicate the position of this new interpolation vector.
Its Axis Definition dialog box appears (see below).
Click OK in the dialog boxes when you are done.

Click to remove the interpolation vector selected in the dialog box.

Click to edit the interpolation vector selected in the dialog box. The Axis Definition dialog box is displayed.

General information about this dialog box is available in the Reference section.

Click OK in the dialog boxes when the interpolation axes are defined.

  8. Set the Machining parameters, for example:
  9. Set the Radial parameters, for example:
  10. Replay the tool path to verify that the tool can be positioned at each point on the trajectory.

If the tool cannot be positioned at each point on the trajectory, adjust the default interpolation axes and possibly insert additional interpolation axes until this criteria is satisfied.

You can add an additional axis by clicking one of the interpolation axis symbols in the Strategy tab page then either selecting an existing point on the part or selecting anywhere on the part.

You can delete an additional axis by right-clicking it and selecting the Remove contextual command.   
You can delete all additional axes by right-clicking one of the interpolation axis symbols in the Strategy tab page and selecting the Remove all additional axes contextual command.
Default axes cannot be removed.

Note that interpolation axes are applied at contact points on the trajectory. The application point of an interpolation axis must be on a selected face. If the point is not on a selected face, it will be projected onto the part. This may give undesirable results.

Once the tool can be positioned at each point on the trajectory, you can set the collision checking option on the Geometry tab page.
  11. If there are collisions detected, adjust the interpolation axes until the tool path is collision free.

Once there are no collisions, you can select the faces of neighboring blades as check surfaces.

You can then replay the tool path to check for collisions with the selected faces.

 
  12. You may need to adjust the interpolation axes and possibly insert additional interpolation axes until the tool path is collision free.

The following figure shows an example of the default and additional interpolation axes that will give a collision-free trajectory.
  The corresponding data is as follows:
Axis Application point coordinates Interpolation axis vectors
1 Intersection point u=0.224917 v=0.0174524 w=0.974222
2 Intersection point u=0.292194 v=-0.0348995 w=0.955722
3 Intersection point u=0.15643 v=0 w=0.987688
4 Intersection point u=0.308264 v=0.0697565 w=0.94874
5 x=-20.8009 y=18.814 z=192.1 u=-0.0688977 v=0.156434 w=0.985282
6 x=23.0488 y=-11.0264 z=192.676 u=0.103351 v=-0.529919 w=0.841727
7 x=12.9556 y=-22.0174 z=252 u=0 v=-0.45399 w=0.891007
8 x=-10.2918 y=16.9498 z=252 u=-0.069714 v=0.0348995 w=0.996956
9 x=-14.1239 y=9.91563 z=192.142 u=0.25878 v=-0.0174524 w=0.965779
10 x=-4.66894 y=1.32628 z=191.888 u=0.207785 v=-0.0348995 w=0.977552
11 x=-5.69227 y=-3.93598 z=192.877 u=0.0347667 v=-0.0871557 w=0.995588
12 x=-20.6779 y=19.1817 z=191.995 u=0.137059 v=0.173648 w=0.975224
  13. The tool path can be replayed and checked for collisions.
14. Click OK to create the operation.
 
  • A default reference tool axis (A) is displayed. You can double click on this axis to modify it. You can also click the tool axis (A) symbol in the Strategy tab page to modify the orientation of the reference axis. This axis is not used in the interpolation.
  • If needed, you can select the Macros tab page to specify the operation's transition paths (approach and retract motion, for example). See Define Macros of an Operation for an example of specifying transition paths on a multi-axis machining operation.
  • If needed, you can select the Feeds and Speeds tab page to specify the feedrates and spindle speeds for the operation.

end of task