Indexing Programs and Index Systems

In this Topic ShowHide

Introduction

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.

Index Systems are only available with the 4 Axis Standard, 4 Axis Pro, 5 Axis Standard, and 5 Axis Pro modules.

Navigation

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.

After creating the first Index system:

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

An index System is created and added to the Machine Setup below the current Index System.

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 System Select dialog box. To select a surface, click Pick a Surface, and click OK. This enables selection mode for you to select a planar surface to assign to the Index System. To use a user coordinate system, click Pick a UCS, select a UCS from the list, and click OK. The UCS is assigned to the Index System. After making a selection, the index system indicator displays and shows the positive (Z-axis) direction for the index. When using a UCS, this automatically uses the positive Z-axis direction of the UCS, but when you select a surface, the direction may need to be changed using the Reverse option.

TIP:   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 - 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.

• Mill 2 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, Swarf 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.

• 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.
• 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.

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

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.)

TIP:   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