Indexing Programs and Index Systems

Introduction

This topic will explain index systems, explain how to access them, and will describe the options found in the dialog. This topic will also explain the options found in the context menu of the index system item in the Machine Setup, and will provide links to related topics.

Index Systems

The Index System defines the rotary angles used for 4- or 5-axis indexing. You add an Index System to define each plane of the part that is machined. To define the plane, you can select a surface or a UCS (user coordinate system). Milling Features can then be created for each Index System. When you use Index Systems, the complete program (including the indexing of the part) can be viewed in simulation.

 

You can also create indexing programs using the Output Rotary Angle option in the Posting dialog box of the Milling Wizard. This method creates proper indexing in the NC program, but the indexing of the part is not shown in simulation.

 

Important: Wrapping Groups are only available with the 4 Axis Standard, 4 Axis Pro, 5 Axis Standard, and 5 Axis Pro modules.

 

To create an Index System:

 

  •  In the CAM Tree, right-click Machine Setup, point to Additional Functions, and click Add Index.

The Index System is created and added to the Machine Setup.


  • Right-click the index system and select Re/Select.

  • The Re/Select Index Location dialog appears to allow you to specify the location and orientation of the index system.

  • Click (OK).

 

After creating the first Index system:

 

  • Right-click Index System, point to Additional Functions, and click Insert Index.

The Index System is created and added to the Machine Setup.


  • Right-click the index system and select Re/Select.

  • The Re/Select Index Location dialog appears to allow you to specify the location and orientation of the index system.

  • Click (OK).

Index System Selection Dialog

Re/Select Index Location - allows you to select an item to use to set the alignment of the indexing system.

 

  • Reverse - will flip the direction of the index system.

Transform Plane Option

 

Use Machine Setting for Posting

 

- will use the posting settings assigned for the machine in the Multiaxis Posting page of the Current Settings.

- will use the posting settings assigned below.

 

Use Transform Plane

 

- will output Fanuc G68.2 or equivalent.

- will not output Fanuc G68.2 or equivalent.

 

Machine Setup Indexing System
   
Use Transform Plane Use Transform Plane



Use Index System Origin

 

- will output the transform plane, and output coordinates from the location of the indexing system.

- will output the transform plane, but output coordinates from its original location.

 

Use Index System Origin Use Index System Origin

The Index System Shortcut Menu

Right-click Index System to access a shortcut menu with the following items.

 

Index System

    • Re/Select - opens the Index Selection Manager. Select either a planar surface or a plane. When you make the selection, the index system indicator displays and shows the positive (Z-axis) direction for the index system. If the default direction is incorrect (not pointing towards the spindle or tool), you can use the Reverse button (or the Reverse command in the shortcut menu). When the direction is correct, click .

 

Important: When you select a surface or plane to set the index location, the surface or plane becomes the Z-axis zero for setting the feature parameters.

 

    • Reverse Direction - is used to flip the Z-axis indicator of the index system when the indicator points in the wrong direction. The index system  indicator should point in the positive Z-axis direction (towards the milling spindle/tool).

    • Mill Drill Hole - opens the Hole Wizard for you to create a Drill Hole feature. This handles drilling with the available operations: Center Drill, Drill, Chamfer Drill, Chamfer Mill, Ream, and Bore.

    • Mill Tap Hole - opens the Hole Wizard for you to create a Tap Hole feature. This handles tapping with the available operations: Center Drill, Drill, Chamfer Drill, Chamfer Mill, Ream, Bore, Tap and Rolling Tap.

    • Mill Counterbore Hole - opens the Hole Wizard for you to create a Counterbore Hole feature. This handles counterbore hole drilling with the available operations: Center Drill, Drill, Chamfer Drill, Chamfer Mill, Ream, Counterbore Drill, and Counterbore Mill.

    • Mill Counterbore Tap Hole - opens the Hole Wizard for you to create a Counterbore Tap Hole feature. This handles counterbore hole tapping with the available operations: Center Drill, Drill, Tap, Rolling Tap Chamfer Drill, Chamfer Mill, Ream, Counterbore Drill, and Counterbore Mill.

    • Mill2 Axis - opens the 2 Axis Wizard for you to create a 2 Axis feature. This handles 2-axis machining with the available operations: Profile Rough, Profile Finish, Pocket, Facing, Engraving, Chamfer Mill, and Plunge Rough.

    • Mill 3 Axis - opens the 3 Axis Wizard for you to create a 3 Axis feature. This handles 3-axis machining with the available operations: Z Level Rough, Z Level Finish, Planar, Spiral, Radial, Plunge Rough, Advanced Rough, Flatlands, Equidistant, and Pencil.

    • Mill 4 Axis Rotary - opens the 4 Axis Rotary Wizard for you to create a 4 Axis Rotary feature. This handles simultaneous 4-axis rotary machining with the available operation: 4 Axis Rotary.

    • Mill Multiaxis - opens the Multiaxis Wizard for you to create a Multiaxis feature. This handles multiaxis machining up to 5-axis output with the following toolpath types: Wireframe, Multiaxis Roughing, Dwarf and the surface-based paths Parallel Cuts, Cuts Along Curve, Morph Between 2 Curves, Parallel to Multiple Curves, Project Curves, Morph Between 2 Surfaces, and Parallel to Surface.

    • Mill Thread - opens the Mill Thread Wizard for you to create a Mill Thread feature. This handles mill threading with the available operations: Center Drill, Drill, Chamfer Drill, Chamfer Mill, Ream, Bore, Pocket, and Profile.

    • Mill 3 Axis Wireframe - opens the 3 Axis Wizard for you to create a 3 Axis Wireframe feature. This handles 3D engraving with the available operations: 3D Engrave Rough and 3D Engrave Finish.

    • V-Carve - opens the V-Carve Wizard for you to create a V-Carve feature. This handles tapered pocketing and V-tool carving using the available operations: Tapered Pocket and V-Carve Finish.

    • Additional Functions - point to this menu item to view the following commands.

      • Update All Geometries - updates all the geometry associated with the feature.

      • Compute All Toolpath - computes the operations of all features contained in the Index System.

      • Insert Index - adds an Index System to the tree after this index system.

      • Insert Wrapping Group - places a wrapping group in the CAM Tree.

      • Add Toolpath Pattern - adds a Toolpath Pattern to the selected Index System. When added from this location, the defined pattern is applied to all of the features in the Index System.

      • Remove - removes the assigned indexing plane from the index system.

      • Delete - removes the Index System from the tree.

      • Delete All Features - removes all milling features in the Index System.

      • Collapse Items - collapses the child items of the Index System. This is the same as clicking the minus sign () next to all child items.

      • Expand Items - expands the child items of the Index System. This is the same as clicking the plus sign () next to all child items.

    • Load Feature - allows you to locate and add a previously saved milling feature to the tree.

    • Paste Feature - is used to paste a copied feature to the Index System after the last feature.

    • Post All Yes/No - sets all toolpaths in the Index System to post or not post in the NC program.

    • Blank/Unblank Toolpath - allows you to hide or show all toolpaths in the Index System.
    • Suppress Toolpath Patten - prevents the child toolpath patterns from being added to the Operation Tree, and does not allow the pattern to be posted.

    • Unsuppress Toolpath Pattern - allows the child toolpath patterns to be added to the Operation Tree, where its individual pattern instances can be set to post, or not post.

    • Rename - enables editing of the Index System name in the CAM Tree. Type the new name for the index.

    • Add Note  - opens the Add Note dialog to allow you to create a message that can be accessed as a tool tip by hovering over the icon next to the item. Click OK to create the note, and use Add Note  again if the note needs to be edited. Editing the note, removing all text and clicking OK removes the note from the item.

Using the Index System

Rotation angles are automatically set in features created using an Index system as long as the proper procedure is followed.

 

The Proper Setup Procedure:

 

  1. Define the stock geometry and Machine Setup for the part.

  2. Add an Index System, and assign the plane for the index system before adding features.

  3. When you add features, you must right-click the Index System (not the Machine Setup) to automatically pick up the proper rotation angles.

 

(If you add a feature from the Machine Setup, the feature isn't added to the Index System.)

 

Note: When you select a surface/plane to set the index location, the surface/plane becomes the Z-axis zero for setting the feature parameters.

Related Topics

How to Create Indexing Programs