About the Model Import Options in the Profiles
The Model tab is the default on the import profiles. The model import options that are available on the Model tab are as follows:
• Use templates—Specifies whether to use the custom start part and assembly template for import of a model. Click Options to select a template for the part or assembly in the New File Options dialog box. You can select the default template models.
If a default profile is not used for the import, you can select the template models specified as the values of the template_solidpart and the template_designasm options.
• Enable ATB—Specifies that file formats that support Associative Topology Bus (ATB) are imported with ATB capabilities. This option is selected by default.
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If the Enable ATB option is not selected during the initial import of file formats that support ATB, the models and features do not have the ATB capabilities after import. The models and features remain without the ATB capabilities even if you select the Enable ATB option in the File dialog box when you subsequently reload or replace the source files or add and redefine geometry.
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• Import type—Specifies the geometric data type of the imported features. You can set the data type of the imported models to one of the following representations:
◦ Geometry—Imports the BREP of the design stored in the selected file for formats such as CATIA V5 CATPart, JT, and Creo View and creates a standard import feature.
◦ Facet—Imports the facet data in the selected file regardless of the filter settings in the import profiles. The facet data is imported as facet geometry or data that generates facet geometry.
◦ Curve—Imports curves or any other data that you can interpret as curves, regardless of the filter setting in the import profile. Creates a curve-from-file import feature.
◦ Automatic—Creates a standard import feature or a facet or curve-from-file import feature, depending on the file format selected for import, the contents read from the file, and the import profile settings. This is the default representation and is not stored with the imported feature or model.
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You can change the import type only during the initial import of the model. If you change the import type of the models when you reload or replace the source files or add and redefine geometry, the imported features ignore the setting and retain their original geometry type set during its initial import.
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• Model Accuracy—Specifies whether to use one of the following model accuracies, regardless of whether you specified the use of the custom start part or assembly template files for the import:
◦ External—Specifies the use of the model accuracy of the source models by default. An external accuracy value is available from the source files. The external accuracy value over-rides the model accuracy of the custom start part or assembly template files. When you import Parasolid or ACIS-based models, the model accuracy of the imported models includes the tolerant edge values.
◦ Internal—Specifies the use of the internally set value of the models as the model accuracy. This value is also set as the default relative accuracy of the models. For file formats such as CATIA V5, this internally set default relative accuracy is a fixed value, such as 0.01 mm.
◦ Automatic—Specifies the use of the model accuracy of the custom start part and assembly template files when the part and assembly template files are used for the import. If the template files are not used for the import, the external or the internal accuracy values of the models are used based on the file format of the model selected for import.
When model accuracy is set to the value Internal or Automatic, formats such as STEP, IGES, and VDA use relative accuracy set to the default value of 0.0012 for import. However, relative accuracy is converted to absolute accuracy during post-import processing in Creo 7.0. That is, models are imported with an absolute accuracy that is based on the relative accuracy set to the value of 0.0012 in Creo 7.0 while models are created with the default absolute accuracy that is available in Creo. However, as relative accuracy is converted to absolute accuracy, the import results of file versions in Creo 7.0 and the file versions of the previous Creo releases are consistent.
Parasolid or ACIS-based models that have tolerant edges, and CATIA V5, import with absolute accuracy. Formats such as NX, SolidWorks, Solid Edge, and the Neutral formats such STEP and IGES are Parasolid or ACIS-based.
• Import facet model as assembly—Specifies whether or not to import a CATIA V5 CGR model with multiple facet bodies as a flat assembly.
The CATIA V5 CGR part components of CATIA V5 CATProduct assemblies import as sub-assemblies when the CATIA V5 CGR components consist of multiple facet bodies. The facet bodies of the CATIA V5 CGR models are imported as individual part components of the sub-assemblies.
When the CATIA V5 CGR part models with multiple facet bodies are not components of CATProduct assemblies, assembly is the default model type in the Import New Model dialog box. Therefore, the CATIA V5 CGR part models with multiple facet bodies import as flat assemblies, especially when you use Creo Distributed Batch for the import. To import the CATIA V5 CGR files with multiple facet bodies as part models, you must explicitly set the model type as part in the Import New Model dialog box.
• Place imported components with aligned CSYS—Specifies whether to import the assemblies with aligned coordinate systems. When cleared, it improves the import performance and the model display.
The following table lists the mapping between the legacy configuration options that controlled the import of 3D model data and the corresponding import profile options:
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Import Profile Options for Model Import
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Corresponding Legacy Configuration Options
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Use templates
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intf_in_use_template_models—yes*, no
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template_solidpart
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template_designasm
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Enable ATB
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topobus_enable—yes, no*
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Import type
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intf3d_in_import_as_facets—yes, no*
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Model Accuracy
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intf_in_external_accuracy—yes, no*
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Import facet model as assembly
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allow_import_faceted_as_asm—yes, no*
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