You can save a part or an assembly as a Creo Parametric neutral (.neu) file. Creo Parametric can read the neutral files with the ATB (Associative Topology Bus) update command to maintain associativity to a previously imported model.
As you update and overwrite the neutral files with a modified model, Creo Elements/Direct Modeling creates corresponding XML files which are required to maintain ATB associativity. Only Creo Parametric can read the neutral files from Creo Elements/Direct Modeling. The files are not compatible with other GRANITE applications.
When you save an assembly, you must specify either a new empty directory or to maintain associativity, the same directory as used in the previous export.
You can export the following part attributes to Creo Parametric:
• Material for sheet metal parts
• Density for sheet metal parts (unit: kg/mm3)
• Thickness for sheet metal parts (unit: mm)
• Volume (unit: mm3)
• Mass (kg)
• You can export feature points that are references of Product and Manufacturing Information (PMI), from Creo Elements/Direct Modeling to Creo Parametric. In Creo Parametric,
◦ A datum point is created for each exported feature point and,
◦ A note is created for the feature point label.
• An annotation between feature points in Creo Elements/Direct Modeling becomes a semantic PMI annotation between datum points in Creo Parametric.
• Feature point references in Creo Elements/Direct Modeling are associative to the model geometry. After the transfer of an annotation that references a feature point to Creo Parametric,
◦ The transferred annotation remains associative to those references.
◦ The transferred references remain associative to the geometry. All exported feature point references in Creo Elements/Direct Modeling do not have a corresponding feature point reference in Creo Parametric. For more information, see
Feature point types.
• If you save a file in the neutral format then the Geometry sharing and GraniteVersion options are unavailable.
• When you import neutral files for sheet metal parts or 3D models in Creo Parametric, disable the ATB to modify the Unit Quantity attribute (volume, mass, and density) and the Unit attribute (mm3, kg, and kg/mm3).
To export to neutral (.neu) file format,
1. Click File > Save in the main menu. The Save dialog box opens.
2. In File Type, select Creo Parametric/Direct Neutral (*.neu*).
3. Click Options. The Write Creo Parametric/Direct dialog box opens. Set the following options:
◦ Click Export Containers to include the containers and their content in the export.
◦ Click Export Face Parts to include the face parts in the export.
◦ Click Export Wire Parts to include the wire parts in the export.
◦ Click Export Empty Parts to include the empty parts in the export.
◦ Click Export Annotation 3D to export 3D Annotations.
• All the 3D annotations exported as a neutral (*.neu) file are created in the tessellated format in Creo Parametric. The tessellated format is a static format that does not have links between annotations and their references.
• 3D annotations are exported only if a model is exported as a neutral (*.neu) file.
• 3D annotation names and references are not visible when you open a neutral (*.neu) file in Creo Parametric.
• Linear dimensions and 3D notes are exported to Creo Parametric with a reference, which could be a point, face, an edge, or a coordinate system.
• For angular dimensions, you should either select an axis or a datum plane of a coordinate system as a reference.
◦ If you select an axis as a reference for an angular dimension in Creo Elements/Direct Modeling, the corresponding axis is referenced for the angular dimension in Creo Parametric.
◦ If you select a plane as a reference for an angular dimension in Creo Elements/Direct Modeling, the corresponding datum plane is referenced for the angular dimension in Creo Parametric.
◦ Click Export Cross Sections to export clipping features and cross sections to Creo Parametric or Creo Direct. For more information, see
Export clipping features to Creo Paramatric.
You can export only those clipping features that are owned by parts or assemblies.
◦ Healing Level: Choose StandardGranite healing level or Extended healing level. The extended healing method considers Creo Elements/Direct specific information.
4. Click Select in the Save dialog box.
5. Select the object to be exported in the viewport or in the Structure Browser.
You can only select a single object (part or assembly) to save in the neutral format.
6. Type the path for the exported file or use Browse.
• You can only specify a directory but not a file name while saving a file in the neutral format. Creo Elements/Direct Modeling assigns a file name, which is derived from the name of the selected object, to the exported file.
• If the selected object is a part,
◦ A .assembly_context.xml file should not exist in the directory.
◦ If a neutral and an XML file already exist in the directory and the SYSID is correct (matching), Creo Elements/Direct Modeling asks if you want to update the files. SYSID is a unique identification (system ID) of an object that associates each pair of neutral and xml files with the selected object. When you save an object, the SYSID of the object is compared with the SYSID in the neutral and xml file.
◦ If a neutral file exists with another SYSID, Creo Elements/Direct Modeling asks if you want to overwrite the neutral and XML files. In this case, an update is not possible as the SYSID belongs to another part.
• If the selected object is an assembly,
◦ If a neutral and an XML file already exists in the directory and the SYSID is correct, Creo Elements/Direct Modeling asks you whether you want to update the files.
◦ If a neutral file exists with another SYSID, choose another directory.
