Translate Mechanical Desktop models to Autodesk Inventor data

Use the DWG/DXF File Wizard to import Mechanical Desktop data, including parts, assemblies and drawings. The data is associative to Autodesk Inventor drawing views and annotations.

1. Select Open.
2. In the Open dialog box, change the file type to DWG files (.dwg), and then select the file to start the DWG/DXF File Wizard.
3. On the DWG File Import Options page:
   • Verify that the file type is Mechanical Desktop.
   • The Default MDT Configuration is automatically selected. Click the arrow to use a different configuration, select the file, and then click Finish.

     To continue setting options, click Next.

4. On the Model Layout/Import Options page, specify the data to translate. Click the tab to enter options:
   • In the Import File Units box, select Detected Units to use a unit setting 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.

     Select Specify Units to convert units to a selection from the list.

   • In the Translate box, Parts and Assemblies is automatically selected. Clear the check box to skip parts and assemblies.

     To translate layouts into Autodesk Inventor drawing views and annotations, select All Layouts as Drawings with Views. Each .DWG file with layouts to translate creates a separate .idw file with one sheet per layout. Not available if Parts and Assemblies is not selected.

     To translate a selected layout into 2D geometry, choose Selected Layouts as Drawings with Draft Views. Requires that a layout is selected before you continue.

5. Click Next.
6. On the Mechanical Desktop Import Destination Options page, click Finish to accept the defaults or set individual options:
   • In Assembly Options, accept Referenced components only or select All Component Definitions.
   • In Part Options, accept As Features and then specify how to translate parts with unsupported features. Optionally, select Translate Body Only.
   • In Drawings with Views Options, accept Selected and External Files or select Selected File Only.
   • In Output Options, specify what to do if a duplicate output file is found. Accept Overwrite or select Use Existing File (to retain existing data).
   • In Templates, accept the defaults or browse to select different templates.
   • In Destination Folder, accept the specified folder or browse to a different folder.
   • In Save to Configuration, browse to select a configuration, if appropriate.
     Note: To save your settings as a configuration to use in the future, save the configuration before you click Finish.

Guidelines for translating Mechanical Desktop data

Note: Migrate files to the latest version of Mechanical Desktop before you translate to Autodesk Inventor. When you open the file in the latest version of Mechanical Desktop (available on the installation CD for Autodesk Inventor), update the assembly, scene and layouts. Then save the file. If necessary, resolve any file links. The migration tool tells you of any data problems so you can repair them before bringing the file into Autodesk Inventor.

• Not all Mechanical Desktop data is translated. Any problems with the translated data are listed in a log file.
• Broken views, base section views, and breakout section views are translated as base views.
• Exploded views are translated as unexploded (no tweaks applied).
• Parametric dimensions (AMPARDIMS) are supported. When AMPARDIMS are present, model dimensions are inferred in the views.
• The Move with Parent option is different in Autodesk Inventor. If Move with Parent is selected in Mechanical Desktop, Autodesk Inventor aligns all views according to the view type.
• If a parent view is deleted in the Mechanical Desktop file, a child view is not created during translation.
• Centerlines and center marks are automatically generated during translation, so they may not be the same as in the Mechanical Desktop view.
• Radial section views have broken alignment.
• Dimensions to apparent intersections are not attached. In Autodesk Inventor, you can reattach the dimension extension lines manually to maintain the reference dimension behavior.
• Dimensions to features that do not fully translate may need to be recreated.

Translation log file

When translating Mechanical Desktop layouts to Autodesk Inventor drawing views, some data may not translate. A log file lists the translation result for each drawing view. When translation is complete a dialog box displays and asks if you would like to view the log file.

The log file name is the combination of the drawing (.idw) file name, the sheet the view is on, and the name of the view. The original Mechanical Desktop DWG file is referenced as well as appropriate assembly (.iam) and part (.ipt) files. The log file has an .xml extension and is located in the same folder as the translated assembly, part, or drawing files.

The log file contains the translation result of each view:

Successful	View and annotations were created with no errors
Successful with errors	A view was created, but it is not the correct view. Or, some annotations were not created or have errors.
Failed	No view was created. Annotations may or may not have been created.

Tip: You can place Mechanical Desktop parts as components in an Autodesk Inventor assembly without importing them.