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DWG Translation

    Table of contents
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    Procedures | References

    When you import an AutoCAD file in Autodesk Inventor LT, or export an Autodesk Inventor LT drawing to AutoCAD format, specify various settings for the translated files.

    To make the process more efficient, you can save a group of settings as a configuration, and use the configuration to set the translation options automatically. You can save as many configurations as needed. Configuration settings are saved in a file with an .ini extension.

    To save a configuration, set the options for opening or saving a DWG (.dwg) file. In the final dialog box, provide a file name and click the Save Configuration before clicking Finish.

    To use an existing configuration, click Browse in the DWG/DXF File Wizard dialog box, and then find the appropriate configuration file. When you specify a configuration file, you do not need to select any other options.

    Note on opening DWG files

    You can set the default behavior for an AutoCAD DWG in the Drawing tab of Application Options. Use the drop-down under Non-Inventor DWG file to specify Open or Import.

    If you do not require AutoCAD objects translated into Autodesk Inventor LT objects, you can directly open any AutoCAD DWG (.dwg) file in Autodesk Inventor LT. You can view, plot, and measure the file contents. Objects display exactly as they do in AutoCAD. In addition, all the AutoCAD data is selectable for copy and paste. You can open an AutoCAD DWG file in Autodesk Inventor LT, and then copy and paste AutoCAD entities into any Autodesk Inventor LT sketch.

    For more information, see Use your AutoCAD geometry.

     

    Procedures

    Use AutoCAD data imported into an Autodesk Inventor LT part or drawing

    In a part or drawing, 2D data is imported into a sketch . AutoCAD 3D solids and surfaces are imported as ASM bodies. If the AutoCAD file contains 3D wire geometry, you can use options to project to a 2D sketch or import as a 3D sketch.

    Note on opening DWG files

    If you do not require AutoCAD objects translated into Autodesk Inventor LT objects, you can directly open any AutoCAD DWG (.dwg) file in Autodesk Inventor LT, and then view, plot, and measure the file contents. Objects display exactly as they do in AutoCAD. In addition, all the AutoCAD data is selectable for copy and paste so you can open an AutoCAD DWG file in Autodesk Inventor LT, and then copy and paste AutoCAD entities into any Autodesk Inventor LT sketch.

    For more information, see Use your AutoCAD geometry.

    Click Open and select the appropriate file. If you are importing a DWG file, click Options. Select the Import option and click OK.

    Click Open to start the DWG File wizard.

    1. In the DWG File Import Options dialog box, continue with one of the following steps:
      • Select a configuration file , and then click Finish. The DWG file is imported with respect to the configuration setting.
      • Click Next to continue setting options.
    2. In the Layers and Objects Import Options dialog box:
      • Select the units.
      • Select Model Space or Layouts (Paper Space). If you select Layouts, only the currently active layout is translated.
      • Select the layers to translate, or unselect the All option and select objects to translate in the preview window.
      • Click Next for more options or Finish to open the file.
    3. In the Import Destination Options dialog box:
      • Under 3D data options, click 3D solids if required. You can enable the options Surfaces and Wires if you select New Part under Destination for 2D data. Click Import into Repair Environment to create a repair node for the imported data. The repair environment provides diagnostic and repair tools for solids and surfaces.
      • Under Destination for 2D data, specify an Autodesk Inventor LT file type by selecting New Drawing, Title Block, Border, Symbol, or New Part. If you select New Part, you can specify the Surfaces and Wires options under 3D data options. You can also choose to import AutoCAD Blocks to Inventor Blocks (see Sketch blocks).
      • Set the destination directory for the new file.
      • Specify how to place dimensions. To place sketch dimensions on a sheet in a drawing file select Promote Dimensions to Sketch. These dimensions are associated with the sketch and change if you move or edit sketch geometry.

        If the check box is cleared, the dimensions are placed as drawing dimensions. Drawing dimensions do not change or control features or part size and are used to document the model.

      • Select drawing and part templates. Set the Sheet Size.
      • To map layers to sketches or map fonts in the translated file, click Mapping Options, and then use the settings in the Mapping Options dialog box.
      • Set the Save to configuration option. If appropriate, click Browse to specify the location where to save the configuration file .
      • Click Finish to open the file.

    Show me how to create surfaces in AutoCAD and import to Inventor

    Import AutoCAD 2D data to a sketch in an existing part or drawing

    Geometry and its associated dimensions are converted to Autodesk Inventor LTsketch geometry .

    Unassociated dimensions, symbols, and other annotations are not imported to a part sketch. In a drawing, the associated dimensions are placed in the sketch with the geometry. Unassociated dimensions, symbols, and other annotations are placed on the drawing sheet.

    Activate a sketch in an Autodesk Inventor LT part or drawing, and then on the Sketch tab, Insert panel, click ACAD.

    In the Layers and Objects Import Options dialog box, set the following options:

    • Select Model Space or Layouts (Paper Space) as the source location for the data. If you select Layouts, only the active layout is translated.
    • Select the layers to translate.
    • Click Finish to import the data.

    Import AutoCAD 2D data to Autodesk Inventor LT data and create a drawing

    AutoCAD 2D geometry is placed in one or more sketches and its associated dimensions are converted to Autodesk Inventor LT drawing dimensions unless you promote them to sketch dimensions. Drawing dimensions do not change or control features or part size.

    Symbols and other annotations are placed on the drawing sheet. Blocks are translated to sketched symbols in the Drawing Resources folder in the browser.

    Click Open and select the file. If you are importing a DWG file, click Options, and select Import options, and click OK. Click Open to start the DWG File wizard.

    1. In the Layers and Objects Import Options dialog box:
      • Select Model Space or Layouts (Paper Space) as the data source location. If you select Layouts, only the active layout is translated.
      • Select the layers to translate.
      • Click Next.
    2. In the Import Destination Options dialog box:
      • In Destination for 2D data, specify New Drawing, New Part, Title Block, Border, or Symbol.
      • Set the destination directory for the new file.
      • Specify how to place the dimensions.
        • Select the check box for Promote Dimensions to Sketch to place sketch dimension on a drawing sheet. These dimensions are associated with the sketch geometry and change if you move or edit the sketch.
        • Clear the check box to place dimensions as drawing dimensions. Drawing dimensions do not change or control features or part size and are used to further document the model.
      • Select a drawing template.
      • To map layers to sketches or map fonts in the translated file, click Mapping Options, and then use the settings in the Mapping Options dialog box.
      • Click Finish to create the file.
        NoteTo use settings in the future, save the configuration file before clicking Finish.

    Import AutoCAD 3D data to a sketch in an existing part or drawing

    1. Open a part file
    2. On the ribbon, click 3D Model tabSketch panel Create 3D Sketch.
    3. On the ribbon, click Sketch tabInsert panel ACAD.
    4. In the Open dialog box, select the DWG file and click Open
      NoteThe Options command is disabled during this step.
    5. In the Layer and Objects Import Options dialog box:
      • Select the units.
      • Select Model Space or Layouts (Paper Space). If you select Layouts, only the currently active layout is translated.
      • Select the layers to translate, or unselect the All option and select objects to translate in the preview window.
      • Click Finish to import the file.
      NoteThe Import Destination Options dialog box is not displayed at this time.
    6. All curve data is placed in the active sketch.

    Import AutoCAD data into a draft view

    When you open an AutoCAD file as an Autodesk Inventor LT drawing, a new file is created. The first sheet in the drawing contains a draft view with multiple sketches. The 2D geometry and text from the AutoCAD file are placed in the sketch associated to the draft view. Dimensions, text, and other annotations are placed on the drawing sheet.

    1. Select Open and select an AutoCAD Drawing (.dwg) file containing 2D data.
    2. Click Options to open the File Open Options dialog box.
    3. Specify a configuration file to set the options automatically. If no configuration exists, specify the settings in the dialog box and click next to continue.
    4. When you have specified all configurations settings, click Finish to open the file.
    5. If the data import dialog box shows errors in the data, click Accept, and then use the Design Doctor to fix the problems.
    6. Use the commands in Autodesk Inventor LT to develop the drawing.

    Save Copy As DWG

    You can use Save Copy As DWG for 2D or 3D files. Save options are based upon the active file type, 2D for drawings and 3D for models.

    This video demonstrates the procedure with a 3D model.

    References

    Import DWG File Options

    Note on opening DWG files

    If you do not require AutoCAD objects translated into Autodesk Inventor LT objects, you can directly open any AutoCAD DWG (.dwg) file in Autodesk Inventor LT. You can view, plot, and measure the file contents. Objects display exactly as they do in AutoCAD. In addition, all the AutoCAD data is selectable for copy and paste. You can open an AutoCAD DWG file in Autodesk Inventor LT, and then copy and paste AutoCAD entities into any Autodesk Inventor LT sketch.

    Specifies options for importing AutoCAD (.dwg), Inventor Fusion (.dwg), or .dxf files. You can save the settings as a configuration for opening other .dwg or .dxf files.

    Access:

    In the Open dialog box, select a file and click Options. Ensure that Import is selected and click OK. Select Open and then click Next in each dialog box to open the subsequent dialog box.

    NoteWhen importing 3D DWG or DXF data to a sketch, the Options command in the Open dialog box is disabled.

    AutoCAD and DXF Options

    Specifies options for opening AutoCAD or DXF files and translating the data to Autodesk Inventor LT files. Click the following choices to display information about the settings in each dialog box.

    NoteWhen importing 3D DWG or DXF data to a sketch, the Layers and Objects Import Options dialog box is not displayed.

    Inventor Fusion Options

    Specifies options for opening Inventor Fusion files and translating the data to Autodesk Inventor LT files. Click the following to display information about the settings.

    Layers and Objects Import Options

    Note on opening DWG files

    If you do not require AutoCAD objects translated into Autodesk Inventor LT objects, you can directly open any AutoCAD DWG (.dwg) file in Autodesk Inventor LT. You can view, plot, and measure the file contents. Objects display exactly as they do in AutoCAD. In addition, all the AutoCAD data is selectable for copy and paste. You can open an AutoCAD DWG file in Autodesk Inventor LT, and then copy and paste AutoCAD entities into any Autodesk Inventor LT sketch.

    Specifies .dwg or .dxf data to translate when importing or inserting an AutoCAD file in Autodesk Inventor LT. You can preview the data in model space or in a layout view.

    NoteThe preview box uses a viewer to display the contents of the specified file. Use the right-click menu in the preview box to access the viewer options and manipulate the view.
    Access:

    Click Open and select the file. If you are importing a DWG file, click Options, and select Import options, and click OK. Click Open to start the DWG File wizard.

    Insert AutoCAD file Select a DWG or DXF file. If you are importing a DWG file, click Options, and select Import options.

    Selective Import

    Specifies layers to include. Select layers to read. To include a layer in the list, select the corresponding check box. Clear the check box to omit the layer.

    NoteEach layer in the AutoCAD file is mapped to a separate sketch in the Autodesk Inventor LT file. To change the layer mapping for the selected file, in the Import Destination Options dialog box, click Mapping Options. Then use the settings in the Mapping Options dialog box.

    Selection

    To select imported objects in the preview window, cancel the All option.

    Color Buttons

    When selected, changes the background color for the Import Preview window.

    Import Preview

    Displays the contents of the specified file for viewing. Use the right-click menu in the preview box to access the viewer options and manipulate the view.

    Import Destination Options

    Note on opening DWG files

    If you do not require AutoCAD objects translated into Autodesk Inventor LT objects, you can directly open any AutoCAD DWG (.dwg) file in Autodesk Inventor LT. You can view, plot and measure the file contents. Objects display exactly as they do in AutoCAD. In addition, all the AutoCAD data is selectable for copy/paste so you can open an AutoCAD DWG file in Autodesk Inventor LT, and then copy and paste AutoCAD entities into any Autodesk Inventor LT sketch.

    Specifies the Autodesk Inventor LT file, file location, and templates to use for translating an AutoCAD file. Available options depend on the settings in the Layers and Objects Import Options dialog box.

    Access:

    Click Open and select the file. If you are importing a DWG file, click Options, and select Import options, and click OK. Click Open to start the DWG File wizard.

    Import Files Units

    Specifies either Detected Units or Specify Units.

    • Detected Units is based on the block insert units (INSUNITS) system variable in the DWG file. If this variable is unitless or set to an unsupported unit, the value of the MEASUREMENT variable (inch or mm) is used.
    • For Specify Units, you select the conversion units from the list.

    Constrain End Points

    Select the check box to apply endpoint constraints automatically or clear the check box to apply constraints in the sketch manually.

    Apply geometric constraints

    Select the check box to constrain the sketch fully.

    Import parametric constraints

    Select the check box to translate AutoCAD 2D parametric constraints to the Autodesk Inventor LT sketch.

    NoteOption available when you select to import Model Space data.

    Proxy objects to user-defined symbols

    Imports proxy objects from AutoCAD to their own user-defined symbols (UDS) in the drawing environment. Not selected by default.

    AutoCAD Blocks to Inventor Blocks

    Select to import AutoCAD blocks as sketch blocks into the Inventor part sketch.

    This option is the default selection when you import an AutoCAD file into an active part sketch. If you import the AutoCAD file into a new part file, the option is available when you select Project wires to 2D sketch.

    Mapping Options

    Opens the Mapping Options dialog box so you can map the layers and fonts in the AutoCAD file.

    Save Configuration

    Saves the settings in the wizard dialog box to box a configuration file that you can use to set options when opening other AutoCAD files.

    Destination for 2D data

    Specifies the Autodesk Inventor LT file type and location for translated AutoCAD data.

    New Drawing creates a Autodesk Inventor LT Drawing file (.idw) and places the 2D data from the specified layers in the new file.

    2D geometry from the DWG file is placed in one or more sketches attached to a draft view.

    • Dimensions are placed on the same sketch as associated geometry.
    • Unassociated dimensions, symbols, and other annotations are placed on the drawing sheet.
    • Blocks are converted to sketched symbols in the Drawing Resources folder in the browser.

    Promote Dimensions to Sketch When selected, places the AutoCAD dimensions as sketch dimensions on a sheet in a drawing file. These dimensions are associated with the sketch and change if you move or edit sketch geometry.

    By default, dimensions are placed as drawing dimensions. Drawing dimensions do not change or control features or part size and are used to further document the model.

    Title Block creates a Autodesk Inventor LT drawing file (.idw) and places the 2D data from the specified layers into a title block.

    Border creates a Autodesk Inventor LT drawing file and places the 2D data from the specified layers into a border.

    Symbol creates a Autodesk Inventor LT drawing file and places the 2D data from the specified layers into a sketched symbol in the Drawing Resources. It then places an instance of the sketched symbol on the first sheet in the drawing.

    New Part creates a Autodesk Inventor LT part file (.ipt) and translates 2D geometry from model space or paper space to an Autodesk Inventor LT sketch.

    • Associated dimensions are added to the sketch.
    • Unassociated dimensions, symbols, and other annotations are not imported.

    Wires to 3D sketch When checked, this option places all wire data in a 3D sketch.

    NoteThis option is enabled only when New Part is selected.

    Project wires to 2D sketch This is the default behavior. When checked, Autodesk Inventor LT projects wires to a 2D sketch.

    NoteThis option is enabled only when New Part is selected.

    Templates

    Part Template Specifies the template to use when creating new files. Use the browse commands to search for and select the appropriate template.

    Drawing Template Specifies the template to use when creating new files. Use the browse commands to search for and select the appropriate template.

    Sheet Size Selects the sheet size from the list.

    Mapping Options

    Maps the layers in the selected AutoCAD file to sketches in the Autodesk Inventor LT drawing or part, and the fonts in the AutoCAD file to Windows or TrueType in the Autodesk Inventor LT drawing.

    Access:

    In the Open dialog box, select a .dwg or .dxf file and click Options. Ensure that Import is selected and click OK. Select Open and click Next in each dialog box to open the subsequent dialog box. On the Import Destination Options dialog box, click Mapping Options.

    Layers

    Maps layers in the selected AutoCAD file to sketches in the destination Autodesk Inventor LT Drawing. By default, a sketch is created for each layer in the AutoCAD file. You can rename the sketches or map multiple layers to a single sketch.

    NoteLayers that are turned off or frozen in the DWG file are not translated.

    AutoCAD Layer

    Shows the layers in the selected AutoCAD file.

    Autodesk Inventor LT Sketch

    Lists the sketches defined for the destination drawing file.

    • To change the name of a sketch, select it, and then type the new name.
    • To map the corresponding layer to another defined sketch, select it, click the arrow, and then select a sketch from the list.

    Map all layers and dimensions to a single sketch

    Maps all layers to a single sketch in the destination drawing.

    NoteMapping a large amount of data to a single sketch can significantly increase translation time.

    Fonts

    Maps the fonts in the selected AutoCAD file to Windows and TrueType fonts in the destination Autodesk Inventor LT drawing. You can map multiple fonts in the AutoCAD file to a single font in Autodesk Inventor LT.

    AutoCAD Font

    Lists the fonts in the selected AutoCAD file.

    Autodesk Inventor LT Font

    Specifies the font to substitute for each AutoCAD font. By default the translator maps to the Windows or TrueType font that most closely approximates the AutoCAD font.

    To choose a different font, click the arrow and select from the list.

    Use Double Stroke

    Adds a duplicate line or stroke to the font in Autodesk Inventor LT to provide a cleaner display for fonts with thin lines. To add the double stroke, click the arrow, and then select Yes. To display the font as single stroke, click No.

    Use Single Stroke Font

    Sets all fonts to use single stroke. Select the box to change the Double Stroke settings for all fonts to No.

    Reset Defaults

    Sets all font mapping back to the defaults.

    .dwg data import mapping

    When you import an AutoCAD file to use in the Drawing Manager environment, 2D entities are translated to corresponding Autodesk Inventor LT entities. 3D data is not translated.

    Note on opening DWG files

    If you do not require AutoCAD objects translated into Autodesk Inventor LT objects, you can directly open any AutoCAD DWG (.dwg) file in Autodesk Inventor LT. You can view, plot, and measure the file contents. Objects display exactly as they do in AutoCAD. In addition, all the AutoCAD data is selectable for copy and paste. You can open an AutoCAD DWG file in Autodesk Inventor LT, and then copy and paste AutoCAD entities into any Autodesk Inventor LT sketch.

    For more information, see Use your AutoCAD geometry.

    DWG data

    Autodesk Inventor LT equivalent

    3D face

    Not translated

    3D solid

    Not translated

    Note3D solids can be translated separately from 2D data.

    Alternate units

    Dual dimensions

    Angular dimension

    Angular dimension

    Arc

    Arc

    Attribute (Attrib)

    Prompted value

    Attribute definition (Attdef)

    Prompted value definitions

    Augmented line

    Line

    Block Definition

    Sketched symbol resource

    Block Instance

    Sketched symbol instance

    Body

    Not translated

    Circle

    Circle

    Color

    Color

    Diameter dimension

    Diameter dimension

    Ellipse

    Ellipse

    External reference (Xref)

    Sketched symbol

    Font change

    Font override

    Group

    Not translated

    Hatch (Associative)

    Hatch

    Hatch (Not Associative)

    Sketched symbol instance

    Layer

    Translated to sketches in drawings.

    Layout

    Sheet

    Leader

    Callout symbol

    Leader arrowheads

    Callout symbol leader arrowhead

    Line

    Line

    Linear dimensions (horizontal, vertical, rotated, aligned)

    Linear dimensions (horizontal, vertical, rotated, aligned)

    Linetype

    Linetype

    Mline

    NotTranslated

    Mtext

    Sketch Text

    Named view

    Not translated

    Ole2frame

    Embedded Excel spreadsheet

    Ordinate dimension

    Ordinate dimension

    Part

    Not translated

    Point

    Point

    Polyline (2D polyline)

    Line

    Polyline (3D mesh)

    Not translated

    Polyline (3D polyline)

    Line

    Polyline (lightweight)

    Line

    Polyline (Polyface mesh)

    Not translated

    Proxy Object

    Exploded and translated

    Radius dimension

    Radius dimension

    Ray

    Not translated

    Region

    Not translated

    Shape

    Hatch

    Solid (2D)

    Hatch

    Spline

    Spline

    AutoCAD surface (such as Stitched, Trim, Extrude, Quilt, Quilted)

    Not translated

    Surface

    Not translated

    Text

    Text

    Tiled viewport

    Not translated

    Title block

    Title block

    Tolerance

    Feature control frame

    Trace

    Hatch

    User Coordinate System (UCS)

    Not translated

    Viewport (paper space)

    Not translated

    Xline

    Not translated

    DWG/DXF File Import Wizard

    The DWG/DXF File Wizard imports parts and drawings with associative relationships with Autodesk Inventor LT drawing views and annotations.

    Note on opening DWG files

    If you do not require AutoCAD objects translated into Autodesk Inventor LT objects, you can directly open any AutoCAD DWG (.dwg) file in Autodesk Inventor LT. You can view, plot, and measure the file contents. Objects display exactly as they do in AutoCAD. In addition, all the AutoCAD data is selectable for copy and paste. You can open an AutoCAD DWG file in Autodesk Inventor LT, and then copy and paste AutoCAD entities into any Autodesk Inventor LT sketch.

    For more information, see Working directly with DWG

    Access:

    Click Open and select the appropriate file. If you are importing a DWG file, click Options, select Import options, and then click OK. Click Open to start the DWG File wizard.

    This dialog box starts the Open DWG File Options wizard.

    The DWG File Import Options page defines options for opening an AutoCAD, AutoCAD Mechanical, Inventor Fusion, or DXF file.

    Configuration

    Selects an existing configuration file to set the File Save Options. Click Browse to find and select an existing file.

    If you select a configuration file, the options are preset in the rest of the wizard dialog boxes. To bypass these options, click Finish.

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