Import Mechanical Desktop Drawings Directly into Inventor 201422 Aug, 2013 By: John Hackney
IMAGINiT Tricks Tutorial: Try this new method to import your Autodesk Mechanical Desktop part files into an Autodesk Inventor assembly model.
Editor's note: This tutorial courtesy of IMAGINiT Technologies.
Many companies started out in 3D design using Autodesk Mechanical Desktop (MDT), but since the software was discontinued in 2009, these files have generally not been used. As designers moved to Autodesk Inventor, there were ways in import MDT files using either their original MDT 2009 software or the Autodesk MDT version for Inventor. When Inventor 2013 arrived, however, this MDT version was not supported for importing files.
Now with the release of Inventor 2014, Autodesk has provided a method to import MDT part files directly into an Inventor assembly model. The part file is added to the assembly as a solid body linked to the original MDT file. It is important to note that the MDT features are not translated into the new part.
To get started, you must modify your Inventor project file. A library entry must be added pointing to the folder containing the original MDT files. You can label it as you desire. Once it's created, right-click on this entry, select Add Proxy Path, and point this to a folder location for the Inventor MDT converted files. If you are using an Inventor Vault project file, these two paths must be outside the project workspace.
The final project file entries will look like the screenshot below. (Of course, your folder names may vary.)
Placing the MDT file into your Inventor assembly is very similar to the process for placing any standard part. Select the Place Component command from the Assembly Ribbon tab or from the right-click menu. In the Place Component dialog box, select the library folder containing the original MDT files.
Select the MDT file you wish to place, then select the Options button at the bottom of the dialog box to make sure the Import option is selected. This setting can be made permanent in the Inventor Application Options under the Drawing tab, Non-Inventor DWG File settings. Select Open to place the part in the assembly.
The files located in the MDT original drawings folder, my MDT folder, are not used after placing in the assembly and can be deleted. The files in the proxy path are used by the assembly and must be retained in order to avoid the Resolve Link dialog box. If you are using the Vault, the original MDT file and the matching proxy Inventor Part file are automatically placed in the mapped folder structure.
Even though the file cannot be edited, all Inventor assembly commands function normally with the file. These functions include constraints, joints, measure, project geometry for new part creation, etc.
How to Make a MDT Inventor Part Editable
If you right-click on an assembly part placed by the above method, you will find that you cannot edit or open it. This is not because it is a library part, but because of the way Inventor imported the MDT file. You can, however, make the part editable by the following process.
Copy the file from the proxy path (in my case, MDT Parts) to any folder within your Inventor project file workspace. This removes it from a library status, allowing you to save your changes. Open the part in Inventor from the workspace. You will notice the 3D Model tab panels in Inventor are grayed out, indicating it is still not editable. Click on the Manage tab and select Make Part. Select the solid body from the browser and configure the dialog box to suit your needs. In my case, I am only creating a new editable part and not placing it into an assembly.
The new part is still a solid body, but it is fully editable, allowing the addition of new features. You also can edit it using a variety of commands. The surface command Delete Face can be used to remove holes, fillets, and chamfers. A little hint: Check the Heal option to get your desired results. The Boundary Patch tool and Sculpt can be used to accomplish the same process. The Move Face command can be used to move existing features to new locations. You can use the Copy Object tool to capture the solid into a surface body or move it into the Repaired Environment to use other editing functions. Inventor Fusion is the tool of choice for these operations, but since it is now an Autodesk Cloud–based application, not all designers will have access to it.
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