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This course introduces you to the interface and key processes of Inventor, the parametric design system from Autodesk. Author John Helfen covers sketching, part modeling, assemblies, and drawings. These tasks work in conjunction, allowing you to create parts and assemblies and document them in a way so that the manufacturing process proceeds faster and more efficiently.
Now that we have our initial views placed, I want to focus on Section and Detail Views. These are slightly more specialized views, and there are not used just frequently as Base and Projected Views, but they are used frequently enough that I want to show you how to create them. Section Views allow you to slice through part so that you can properly document the inside components of a part. We're going to zoom in and create a section of this view. There's a couple ways to begin. From the Place Views tab under the Create panel, we could select Section, and you'll notice in the bottom left-hand corner the Status bar is telling us to select a view or view sketch.
If I hover over the view and left-click, it tells the system that this is the view we want to create the section from, and we can continue on creating our section line. I'm going to hit Escape on the keyboard to cancel this command. The other way to do this is to actually use the Marking menu. If I hover over the specific view I want to create a section of, right-click, I can select section from the Marking menu itself. This does two things, it launches the command, and it selects the view we want to create the section from all in one action.
Now that we're in this Section view command, we need to essentially draw a line that represents where we want the cut to take place. I want is part to be sectioned right down the middle of this hole. So I'm going to hover over the midpoint of this top line, and I'm going to use the Alignment Indicator to position my start point for the line. I'm going to left-click, and as I drag my cursor down below the part, you'll notice I get a perpendicular indicator at that location. This is telling me that this section line is going to remain perpendicular to the initial line that we hovered over to get our midpoint.
I'm going to left-click to place the endpoint of the line. If I wanted to continue on making more sections and maybe a more advanced part, I could do so, but I'm ready actually to create this section line now. I'm going to right-click on the screen and select Continue. When I do that, the Section view dialog box comes up, and Inventor creates a preview of the view. If I drag the view back and forth across the part, you'll notice that the section line automatically changes based on the location of my cursor. I'm going to go ahead and position this off to the left and talk a little bit about the dialog box.
Within the dialog box, we have the ability to make some basic changes. We can change the Label Identifier, we could change the Scale, and even the Style. In case of this section we can also change from a Full section to a specific Depth or Distance, but in this case I'm going to go ahead and leave the Full. So the default settings work perfectly for me. I'm going to go ahead and left-click to place this view. After doing so, Inventor renders it as a Section view. It also applies the hatch automatically based on the material type, it's also created a label for us, it's provided our scale, and it's labeled the section line so that we can quickly identify where the section was created from.
Next, I want a little bit about the Detail view. Detail Views are created in a very similar fashion to the Section Views, so this makes perfect sense to combine the two. Say, for example, we want to get a little more detail of this lip here up from the section. To do so, we can use the marking menu just like we did with the Section view, right-click on the view, and select Detail view. Just like the Section view the Detail view dialog box is presented, and we have the ability to change the Identifier, the Scale, the Style, and a few other options.
At the most basic level, the default settings are going to work most of the time. So I'm going to go ahead and begin creating my detail view. To actually create the detail view, you need to left-click in the center of where you want your detail view to begin. In this case, I left-clicked right in the middle of that lip that I want to detail. Now as I drag my cursor, I can adjust the size of the detail and the position of the label for this detail. Right about here looks about the right size. I'm going to go ahead and left-click to create the view, and Inventor creates a preview.
I can now zoom out, find a position on my drawing sheet where I want to place this view, and left-click to create the view. Just like the section view it provides a detailed label, it provides a scale label, and it labels the initial detail view so that you can quickly determine where this detail is coming from. One last thing about the Detail view: Sometimes you're going to find that maybe the detail changes or the part changes, and you need to reposition this detail. You can do so by simply hovering over the detail indicator, clicking and dragging the position of that circle.
By doing so, the Drawing view updates automatically to show the new position of the Detail view. This comes in handy when the part changes or if for some reason you made an improper selection. You don't have to start from the beginning. You can just reposition this Detail view. Now that I've zoomed out a bit, you can still see that my Section view is little off from a position standpoint, and I'm going to simply drag that over so it's a little further away and my views are a little bit more aligned. I'll even adjust my position of my Detail view a bit.
Now I've got a nice, clean position for my Drawing Views, and I can continue on documenting my design.
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