Inventor

Use Part Design View Representations in Autodesk Inventor

23 Aug, 2012 By: Mark Flayler

IMAGINiT Tricks Tutorial: Part representations can help you with assembly constraints and model documentation.


Editor's Note: This tutorial courtesy of IMAGINiT Technologies.

When modeling parts and building design intent from the bottom up, it is often necessary to reference certain criteria from the part model for use in assembly constraint creation as well as documentation of a model. Introduced in Autodesk Inventor 2012 and enhanced in the 2013 version, part design view representations aid these processes in many ways.

Taken from the idea of assembly view representations, part representations exist in the Model Browser and can include elements such as sketch visibility, work plane visibility, color, and solid body visibility (in Inventor 2013). Here we will take a look at general assembly usage of the view representation, as well as multibody part modeling documentation.

Part Design View Creation

To create a new design view, we start the same way as we do in an assembly: Right-click on the View node in the Model Browser and select New. Once it's created, give it a better name than View1.



In the new design view, toggle any work features, sketches, or model appearance options that you want to save for later use. Typically work feature visibility is a popular one, since we would like to control this on a part-by-part basis when we are working with constraints in an assembly. Having too many planes turned on can create confusion when selecting the correct planes for the Constrain or Assemble command. For this example, we will use simple color change in our representations, since our part numbers for this design are not color-dependent.



Once you have a design view created in the manner you wish to save it, simply right-click on the view and choose Lock to keep it from changing.

General Assembly Usage

Based on your type of usage, you could be using part design views to control color or visibility of work features inside an assembly. To enable a design view of a part inside an assembly, simply locate the file and expand the node on the part. Choose the Representation option by right-clicking on the View node in the expanded tree of that part file.



This will bring up a Representation dialog box so you can choose which design view is appropriate for the task at hand.



The Associative button works the same way here as it does with Presentation files and drawing files. If you want your assembly and its part to update based on changes made to design views in the parts, you must select the Associative option; otherwise they will take on a point in time reference of that design view.
 


Note: By default, Inventor 2013 will always bring in the Last Active option when placing parts into an assembly. To change this on a case-by-case basis, you may select options before placing the part from the Place Component command. If you want Inventor to always bring in the Master Part View (which I recommend), you may select it in the Application Options. Navigate to the File tab and select the Options button in the File Open section of this tab. This will launch another dialog box, where you can select default File Open options for various file types.



Part design views can also be stacked into assembly design views. In the image below, you can see that Sideplate: 1 has a Constrain Planes view representation active, and Final Mold Assy.iam also has this view representation set. They do not automatically link, however, so this would be a conscious adjustment for you to make when setting design views. In this example, we have design views that would turn on for constraining usage without the user having to dig into each file and locate each plane. The only drawback to this is that the origin planes do not currently work with part design views, so you may have to make offset planes of 0 magnitude from the origins and use those instead if you like this approach.



Documentation Usage

When these part design views were introduced in Inventor 2012, they did not work with solid body visibility. Ever since Inventor 2010, when multibody design was introduced, users have been trying to make drawings without having to first use Make Components or Make Part commands to segregate the files into separate modeling files in order to document. Some designs were better left as a multibody part file, especially during the concept stages of design. With Inventor 2013, you can now control solid body visibility in part design views as well as directly in the drawing environment.



When placing the view of the multibody part into the drawing file, you will also have the option to choose which design view to place from the base view command. Remember to use the Associative option here as well, if you desire.



You may now document design views for each individual solid, or if you want to group solid bodies together for documentation of the design in your drawings.


About the Author: Mark Flayler

Mark Flayler

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