You can open an IGES file in Autodesk Inventor (creating a file), import an IGES file into an existing Autodesk Inventor part file, or place an IGES solid body as a component in an assembly.

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.

Procedures

Import and use IGES data

You can import an IGES file to a new or existing Autodesk Inventor part. The imported data can be used as construction surfaces, wires, or the basis for a part.

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 Manage tabInsert panel Import 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.

Open an IGES file in Autodesk Inventor

When you open an IGES file, Autodesk Inventor creates a file and places the IGES data into the new file.

Click Open.
In the File Open dialog box, set the Files of type to IGES.
Select the file and then click Options. In the Import Options dialog box:
- Specify the Part and Assembly Destination Directories if you want to change the defaults.
- Select from Solids, Surfaces, Wires, and Points as Entities to Import.
- If importing surfaces, select Construction Group Mapping to import the data into the construction environment. Select Auto Stitch and Promote to combine surfaces with matching edges into a quilt and promote to the part environment.
- Specify whether you want the data mapped in single or multiple construction environment groups, or directly as composite features. Indicate if the collections are to be created from levels or groups. If appropriate, you can append a prefix to group names, such as the origin file name.
- Choose from the applicable Options and Post Translation Options.
Click OK to close the dialog box and then click Open to import the IGES file using the specified settings.

Import an IGES file into an Autodesk Inventor part

Open the destination Autodesk Inventor part file or create a part file.
On the ribbon, click Manage tabInsert panel Import.
In the Import dialog box, set the Files of type to IGES.
Select the file, and then click Options. In the Import Options dialog box:
- Select from Solids, Surfaces, Wires, and Points as Entities to Import.
- If importing surfaces, select Construction Group Mapping to import the data into the construction environment. Select Auto Stitch and Promote to combine surfaces with matching edges into a quilt and promote to the part environment.
- Specify whether you want the data mapped in single or multiple construction environment groups, or directly as composite features. Indicate if the collections should be created from levels or groups. If appropriate, you can append a prefix to group names, such as the origin file name.
- Choose from the applicable Options and Post translation options.
Click OK to close the dialog box, and then click Open to import the IGES file using the specified settings.

Place an IGES file into an Autodesk Inventor assembly

Open the destination Autodesk Inventor assembly file or create an assembly file.
On the ribbon, click Assemble tabComponent panel Place.
On the Place Component dialog box, set the Files of type to IGES.
Select the file and then click Options. In the Import Options dialog box:
- Specify the Part and Assembly Destination Directories if you want to change the defaults.
- Select from Solids, Surfaces, Wires, and Points as Entities to Import.
- If importing surfaces, select Construction Group Mapping to import the data into the construction environment. Select Auto Stitch and Promote to combine surfaces with matching edges into a quilt and promote to the part environment.
- Specify whether you want the data mapped in single or multiple construction environment groups, or directly as composite features. Indicate if the collections are to be created from levels or groups. If appropriate, you can append a prefix to group names, such as the origin file name.
- Choose from the applicable Options and Post translation options.
Click OK to close the dialog box, and then click Open to import the IGES file using the specified settings.

Stitch and promote imported IGES data

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.

To place all data from an IGES file in a single part, regardless of the 308/408 definitions, use Manage tabInsert panel Import to place the data into an existing file.

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.

References

Import STEP or IGES Options

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.

Access:

In the Open, Import dialog boxes:

Set the Files of type to IGES or STEP.
NoteYou cannot import STEP files using the Import dialog box.
Select or browse to the IGES or STEP file.
Click Options.

NoteIf you choose to translate a file using the Import command, some import options are not available.

Save Options	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. NoteSpecify file destinations that are included in the active project or add the paths to the project to assure that referenced files resolve when you open a file.
Translation Report	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.
Data Organization	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: Single Composite Feature to import the assembly as a single composite feature in the part environment. Multiple Solid Part to import the assembly as individual solid bodies in the part environment. 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: Individual Surface Bodies to import each surface as a single surface body in the part environment. Single Composite Feature to import the surfaces as a single composite in the part environment. Multiple Composite Features to import the surfaces as multiple composites in the part environment. Composites are created for each level, layer, or group, as defined by the Create From selection. Single Construction Group to import the surfaces as a single group in the construction environment. Multiple Construction Groups to import the surfaces as multiple groups in the construction environment. Construction groups are created for each level, layer, or group, as defined by the Create From selection. 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.
Units	Import Units. Converts the imported geometry and parameter values to the selected units.
Post Processes	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. NoteThis option may significantly increase the amount of time required to translate a file. 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.

NoteBy default, Autodesk Inventor applies the part name (file name of the inserted part) to browser file nodes. Other CAD systems might apply the part number property. When a STEP file is imported into Autodesk Inventor, its name might differ from the name of the CAD system which generated the STEP file. To avoid confusion, use the Rename Browser Nodes command to specify the browser node naming scheme.

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Import and use IGES data

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