Embracing Different Views1 Aug, 2003 By: Jeff Wymer
Autodesk Inventor can automatically create 2D drawing views from the 3D models you create. In this column we'll cover the basics of creating these drawing views--everything from simple orthographic projections to section, break out, and broken drawing views.
When you create a new drawing in Inventor, you need to create the initial drawing view from which you'll create subsequent views. The initial drawing view is called the base view. You can right-click in the drawing background and select Base View or select the Base View icon from the panel bar. Base View will open the Drawing View dialog, which allows you to specify the view scale factor, whether to display or remove hidden lines, whether to display a shaded drawing view, and which part/assembly file to use to create the drawing views. If you use an assembly file to create drawing views, the Design View option becomes available, which can create a drawing view based on a predefined design view in the assembly. This drawing view can then be updated based on changes to the design view in the assembly. The scale factor and view orientation are defined prior to placing the base drawing view. The View Orientation pulldown has all the predefined, standard view orientations. If none of the predefined options works for you, you can define a custom view orientation by choosing the Change View Orientation icon beside the pulldown list, as shown in Figure 1. After all the options are defined, select an area on the drawing sheet to place this first view. Inventor will do the rest.
Figure 1. If you cannot find a predefined view orientation that fits your needs, you can define a custom view orientation using the Change View Orientation icon situated beside the pulldown list.
Creating orthographic projections is as easy as 1, 2, 3. The easiest way to create additional views from the base view is to right-click anywhere in the view area (the border around the base view will become highlighted in red) and use the Create View and the Projected options. Select the orthographic projection by dragging you mouse: drag to the right for a right-side view, drag it up for a top-sided view, drag to the left for a left-side view, and so on. The Projected View command keeps repeating. When you want to terminate the command and create the views, right-click and select Create. Since these views are defined from the base view, they automatically inherit the same view properties, such as hidden-line display and scale factor. If you want to override any of the view properties, you can edit them by double-clicking in the view to activate Edit View, or by right-clicking and choosing Edit View. To change the default projected views, you'll need to uncheck the Style From Base option.
You create the section cut-line by sketching the section line during section view creation. When sketching the cut-line, you can inference constraints from the geometry within the view. The inferencing and the sketching of the cut-line is the same as sketching in the part-modeling environment. If you create the cut-line without constraining it to the geometry within the view, you'll be able to drag or move the cut-line to different cut locations after the view is created. If you create the cut-line by inferencing or constraining it to other drawing geometry, the cut-line location will always update based on geometry changes. The section view types supported in Inventor are full, half, offset, and aligned. The creation methods and section view types are the same whether you're creating a part section view or an assembly section view. If you need to change the hatch pattern or scale factor, simply right-click on the hatch pattern and choose Modify Hatch. Here, you can change the pattern type, scale factor, color, angle, and line weight. The default hatch pattern is predefined in the default standards, which can be accessed via the Format pulldown menu, Standards option, and the Hatch tab.
When creating section views of assemblies, you may need to remove components (for instance, fasteners, shafts, bearings, and so on) from the section view. This can be easily accomplished by tagging the components in the parent view to indicate they are not to be sectioned. To do this, you can reveal the components in the browser by right-clicking on the parent view and selecting Show Contents. This will expand the browser to show the entire assembly structure. You can now select the components that you do not want sectioned in the browser, right-click, and uncheck the Section option, as shown in Figure 2. It's very important that you uncheck section in the parent view--not in the section view itself. You can also toggle the Remove from Section by changing your selection filter to Select Part. This enables you to select the components in the graphics window and right-click to access the Remove from Section option. Other views can be projected from a section view.
Figure 2. When creating section views of assemblies, you may need to remove unwanted components from the section view. One of the methods you can use is to select the components you do not want sectioned, right-click, and uncheck the Section option.
Break Out Views
This view allows you to remove a defined area of material to expose obscured parts or features in an existing drawing view. To create a break out view, create an enclosed sketch in the parent view that will define the break out area. This sketch can use any sketch elements, including splines and ellipses. Once you've defined a sketch, you can create the break out view by right-clicking in the parent view and choosing Break Out. The Break Out View dialog box should automatically select the sketch previously created to define the break out area. Now you simply choose from one of the four break-out methods: From Point sets a numeric value for the depth of the break out; To Sketch uses sketched geometry associated with another view to define the depth of the break out; To Hole uses the axis of a hole feature in the view; Through Part uses the thickness of a part to define the depth of the break out (which is useful in creating a break out view of an assembly).
This creates a broken or foreshortened drawing view, especially useful when documenting very long components. To create a Broken View, you simply click and drag the broken length you want removed from the view. During the process, you have control over the broken style: (whether it is rectangular or structural, which structure is used, and so on). You can change the orientation of the broken element, making it either vertical or horizontal, and you can change the distance between the breaks by using the gap value. Symbol controls the number of breaks in a structural style broken view.
A detail view allows you to scale a selected area of a drawing view to further document your design. There may be a very small section of your design that's difficult to annotate due to its intricacies. When creating a detail view, you select an existing view as the parent view. In the Detail View dialog you can set the detail label, the display style of the view, and the scale factor for the view. Once this information is defined, select the area in the parent view that'll serve as the center of the detail, and drag your cursor to define the detail view boundary. You can now select the desired location on the screen to place the view. Since this is not a projected view, it does not need to be inline to the parent view. If you need to move the detail view label, you can simply drag it with the mouse to a new location around the detail circle. You can also redefine the detail circle location and size by dragging the detail circle itself.
You can create an auxiliary projection by selecting an edge to create the projection from. The auxiliary view will be created perpendicular to the selected edge. Inventor will project the entire view--not just the face. If you require an auxiliary view of just the face, you can create a section view where you define the section cut-line to be only the face for the auxiliary view.
Automating the tedious and time-consuming process of creating orthographic projections and drawing views allows you to create drawings that may have taken you hours or days in the past in a fraction of that time.
Autodesk Technical Evangelist Lynn Allen guides you through a different AutoCAD feature in every edition of her popular "Circles and Lines" tutorial series. For even more AutoCAD how-to, check out Lynn's quick tips in the Cadalyst Video Gallery. Subscribe to Cadalyst's Tips & Tricks Tuesdays free e-newsletter and we'll notify you every time a new video tip is available. All exclusively from Cadalyst!
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