To Create a Publish Geometry Feature
1. Retrieve an assembly or a part.
2. For an assembly, click Tools > Publish Geometry. For a part, click Model > Model Intent > Publish Geometry. The Publish Geometry dialog box opens.
3. Select the type of reference elements on which to base the feature and add references.
You can only select elements of the model that owns the Publish Geometry feature (assembly, subassembly, or part). Unlike Copy Geometry and external Copy Geometry features, Publish Geometry features cannot reference other Publish Geometry features.
You must define at least one of the following reference elements to complete the Publish Geometry feature:
Surface Sets—Select surfaces.
Bodies—Select bodies in an activated or open part. Body properties are included in the Publish Geometry feature.
You cannot use a Publish Geometry feature with bodies as a reference for a Copy Geometry feature in an assembly.
To create a Publish Geometry feature that includes all bodies in the part follow the steps below:
1. Click the Bodies collector.
2. Select the part in the Model Tree, or in the graphics window. (To select from the graphics window set the selection filter to Part.)
Chains—Select edges or curves. This collector is used to select a surface or quilt by defining the boundary of the surface or quilt.
References—Select various reference features.
Annotation—Select various annotation features: notes, symbols, surface finishes, geometric tolerances, reference dimensions, and driven dimensions with tolerances.
4. Click Details to add a rule for reference collection, view, add, or remove a reference from the list of references.
5. Click Properties to change the default, feature name.
6. Click OK. The new Publish Geometry feature, identified by the visual indicator, appears in the Footer of the Model Tree.