When you open an IGES file, 308 and 408 structures are used. The block structures in the file are translated into multiple parts referenced by an assembly. Each part file contains the data for a single structure instance.
When you use Open and select an IGES file, click Options to set import options. On the Import Options dialog box, specify the data to import and other conditions to be applied.
Choose the data to import by selecting Solids, Surface, Wires, Points, or any combination.
If the Import into Repair Environment option is selected, the imported data is placed in the browser as a repair body composite.
If the Composite Feature Mapping option is selected, the imported data is placed in composites.
If the Construction Group Mapping option is selected, the imported data is placed in a Construction folder that contains individual group, solid, surface, and wireframe nodes. Surfaces are contained in a single node to help manage them for promotion in Part modeling. You can promote multiple surfaces as a single feature.
Composite features have the same behavior as Base Surface features, but they can also have multiple individual solid and surface bodies within them. While the composite can contain multiple bodies, you cannot work directly with the individual bodies. You can only interact with the composite as a whole.
If possible, multiple surfaces are stitched together into a single part. If edges do not match exactly, the surfaces are stitched into the smallest number of quilts possible.
Surfaces that cannot be stitched together remain in the Construction folder in the browser. Quilts are promoted to the part environment and are shown as surfaces in the browser. In the construction environment, you can analyze and repair surfaces that did not automatically stitch when they were imported.
When opening an IGES file that contains 308/408 subfigure (block) definitions, an assembly file is created using the 308/408 (block) figures to define the assembly structure. If the Auto Stitch and Promote option fails or is turned off, the data is placed in construction groups in the defined part.
Optionally, you can ignore the 308/408 subfigure (block) definitions and open all the data into a single part file. To do this, open a new part and click the Insert menu, and then click the Import option to import all the data into the new part doc.
Use Place Component and set the file type to IGES to place an IGES file directly into an Autodesk Inventor assembly as a solid body, surfaces, or wireframe data. In an open part or assembly file, use to place an IGES file.
Use the Auto Stitch and Promote and the Enable Advanced Healing options to clean up the data as it is imported. The Check Parts on Import option can also be used to determine quality issues during the import process.
If an IGES file contains 304/408 subfigures, it is opened as an assembly. Auto Stitch and Promote automatically stitches and promotes surfaces for each of the resulting parts, if possible. When the assembly is opened, all data placed in the construction environment for each of the parts is not visible in the assembly. Activate individual parts to stitch and promote. Once the data is imported, it is visible in the assembly.
Specifies the import criteria for imported STEP or IGES files. Specifies the data types to import and how data are grouped in Autodesk Inventor. A translation report is generated that includes information on the imported data and its quality, as well as a list of the parts and assemblies that were created in Autodesk Inventor.
In the Open, Import dialog boxes:
Save Components during Load. Select the check box to save the assembly and part files in Autodesk Inventor format during the import process. Choose where to save the components from the drop down menu. If you choose to Select Save Locations, the Component Destination Folder and Place Top-level Assembly in Separate Folder become available. This setting is not available when the Import command is used.
NoteSave Components during Load minimizes memory consumption by saving each component to disk during the import process. If you import larger assemblies and experience long import times or import failures, use this option to reduce memory requirements. For smaller assemblies, the increased process time required to save each component to disk can offset the benefit of improved memory utilization.
Component Destination Folder. Sets the location for the part and assembly files created from the import operation. If Save in Workspace is selected, this folder is defined in the Edit Projects panel.
Place Top-level Assembly in Separate Folder. Select to save the top-level assembly file to a location different than the part files. If Save in Workspace is selected, this folder is defined in the Edit Projects panel.
Embed in Document. Select to display the translation report icon , under the 3rd Party browser node , in your new file. To view the translation report, double-click the report icon, or right-click and select Edit.
Save to Disk. Select to save a copy of the report to disk. Under Save Options, if Place Top-level Assembly in Separate Folder is selected, the translation report is stored along with the top-level assembly. Otherwise, the report is stored in the Component Destination Folder.
Entity Types to Import
Solids. Select to import solid bodies and water tight stitched shells as individual solid bodies.
Surfaces. Select to import surface bodies. Water tight stitched shells are imported as solid bodies.
Wires. Select to import wires.
Points. Select to import points.
Import into Repair environment. Select to check the model for errors and create a repair node in the browser. You can edit, diagnose, and repair an imported base body in the Repair environment. A repair body participates in the model history.
Import Assembly as Single Part. Select to import the assembly as a single part. Choose from:
This setting defaults to on and is not selectable when the Import command is used.
Create Surfaces As. Select the surface types to create during the import. Choose from:
NoteEnable the Construction Environment on the Part tab in the Application Options to make Single Construction Group and Multiple Construction Groups available.
Create From. Specify Levels (Layers) or Groups from which to create Multiple Composite Features or Multiple Construction Groups. Available when the Create Surface As selection is Multiple Composite Features or Multiple Construction Groups.
Add Prefix to Group Names. Select to add a prefix to the source file group names. For example, if the source file has a group Surfaces1 and you define INV_ as the prefix to add, the translated group becomes INV_Surfaces1. Available when the Create Surface As selection is Multiple Composite Features or Multiple Construction Groups.
Group Name to Place Data. Select a Group Name under which to place the imported data. The group name is shown in the browser.
Import Units. Converts the imported geometry and parameter values to the selected units.
Check Parts during Load. Select to perform a quality check of the imported data. If a bad data is found, the composite is marked with in the browser and the remaining bodies are not checked.
Auto Stitch and Promote. When selected, Autodesk Inventor attempts to stitch surfaces into a quilt or solid. If the surfaces are stitched into a single quilt or body, the resulting quilt or body is promoted to the Part environment. Otherwise, the surfaces remain in the Construction environment.
Enable Advanced Healing. If selected, slight alterations in the surface geometry are allowed to stitch the surfaces.