Tutor for CATIA Assembly: Product Specification Tree

Product Specification Tree

Overview: In the Assemblies workbench, the Specification Tree is referred to as the Product Specification Tree. It displays the assembly as a tree structure with nodes that allow you to quickly determine the active component and loaded components.

Product Specification Tree

The Product Specification Tree contains a tree structure representation of the assembly. Each component in the assembly's tree displays as an entry, or node. Use these nodes to select components as you would in the Graphics window, whenever CATIA prompts you for a selection.

Using the Product Specification Tree

Use View | Specifications, or press F3, to access the Product Specification Tree. If the structure is too large for the window, you can use the scroll bars to pan up and down to view the rest of the structure. You can also move it to a different location in the Graphics window. If you click on a white branch, you can resize the tree by using your preferred technique to zoom in and out.

Tree Display

The assembly structure displays as a tree. Each component, whether a piece part or sub-assembly, is indented. Each indentation represents a level in the structure. When you place the cursor over a piece part node and click, the component highlights in both the Graphics window and the Product Specification Tree. Understanding the tree structure and symbols makes it much easier to work with assemblies.

Tree Symbols

CATIA uses several different symbols in the Product Specification Tree, and it is difficult to remember them all. The differences between some of the symbols can be very subtle. For instance, the gear in the symbol may be green instead of yellow. In addition to these symbols, CATIA often uses graphic modifiers to indicate the state of an object. Rather than list every variety, we provide a sample of the more common symbols and modifiers.

Product
Indicates a product. The paper in the icon indicates that this product is saved in its own .CATProduct file.
Component
Indicates a component in this assembly. Since there is not a piece of paper in this icon, this component is not saved in its own .CATProduct file. This sub-assembly only exists within the current assembly, and it cannot be saved separately.
Flexible Sub-Assembly
Indicates a flexible sub-assembly by displaying a purple gear in the symbol.
Instance of a Part
Indicates an instance of the part in the product assembly file. The red Y symbol (which is a coordinate system) means that there is a geometrical representation of the part. If the Y symbol is gray, the node has been deactivated. To restore the geometrical representation, highlight the node and select Edit | Representations | Activate Node.
Reference of a Part
Indicates a reference of a part. This icon displays one level below the instance of a part in the Specification Tree. It shows that only a reference to the part exists in the assembly file and not the actual part itself.
Part Body
Indicates a part body. Click the plus symbol to expand the tree to access individual part features.
Constraints
Displays when constraints exist in the assembly file. Click the plus symbol to expand and view them. Depending on the assembly structure, there can be numerous constraint symbols relating to sub-assemblies present.
Publication
Indicates a published element. Constraints that use published elements are more robust to part changes and revisions than constraints that use the part geometry directly. CATIA shows published elements of the top-level assembly by creating an extra node in the Specification Tree at the top level.

Status

Throughout the Assembly Design process, it is useful to know the status of your assembly. CATIA provides variations of standard symbols in the Specification Tree, which can give you valuable information about the assembly and its components. You can tell whether a component is out-of-date or if constraints are broken due to a modification.
No Visualization of the Product
Indicates CATIA cannot find any reference to the assembly product.
Broken
A graphic modifier that indicates a broken link. CATIA can't find the source information for the entity.

Broken Link
Indicates a broken or lost link between the product and a reference document. You need to re-link the data.
Broken Constraint
Indicates a broken or lost constraint. You need to reconnect the constraint or delete it.
Deactivated
Indicates that the object is deactivated.
Deactivated Constraint
Indicates a deactivated constraint, in this case a parallelism constraint.
Deactivated Component
Indicates a deactivated component. The component disappears from the Graphics window. To reactivate, pick the component in the Specification Tree and select Edit | [ component ] object | Activate / Deactivate Component.
Update
Indicates the object is out-of-date and needs to be updated.
Update Component
Indicates an out-of-date component that needs to be updated. If automatic updating is not activated in the Assembly Design options, you need to update the component manually by picking it and selecting Edit | Update.
Product Hidden
Indicates a hidden object when any symbol has a gray overlay or background. To show the object again in the Graphics window, click on it and select View | Hide/Show | Hide/Show.