Join John Helfen for an in-depth discussion in this video Create section views, part of Autodesk Inventor 2018 Essential Training.
- [Voiceover] Let's take a minute and look and how we can create a section view of our engine block. A section view is essentially just a lined review that allows you to split the part open and see the inner workings of the part or assembly. The way you create one is very similar to a projected view with one additional step, and that's to create a section line. To continue, we need to go to the Create panel on the Place Views tab, and select Section. You'll see in the status bar down at the bottom of the screen that Inventor wants you to select a view just like you did in a projected view. You need a parent or base view to work from. And we're going to hover over this until the red dotted line shows up, and then left click.
That'll tell Inventor that that's the view you want to use as the base, and here in the status bar you can see it says Enter the endpoints of the section line. To do that, we're going to zoom in a little bit so that we can more clearly see our drawing. And at this point, we're just sketching like we were in part modeling almost. What we're going to do is hover near the midpoint of this line at the top, and you'll see a green dot indicating we found the midpoint. Now in the sketching world, if you were to move away from this and see the alignment, and create a line there, it wouldn't create a constraint. In the section view, it does create a constraint cause it makes it a little bit easier to lock it to the part so that you know your section's going to run through that location at any point.
We can simply left click, that starts our line, drag straight down, and you'll see a parallel icon next to the cursor, indicating that it's picked up a parallel to one of the vertical edges. We can left click to locate the endpoint and then simply right click and select Continue. Once we do that, the Section View dialog box comes up and you should recognize some of this, it looks like the settings that we had in the previous movie. We can change the identifier or the label, we can change the scale, we can also change the style from hidden line to hidden line removed, or even add shaded.
What I'm going to do is simply move over on drawing view and left click to place that view. Here you can see the section view is created, the section lines labeled F-F, the section view is labeled F-F and it includes the scale. Let's take a minute to look at how we can create an offset section. We're going to go ahead and return to the Create panel and select Section one more time. We're going to select the view we want to start from, we'll select the same one we started last time. But this time, rather than creating a line straight through, we're going to create an offset section.
We're going to start in the same manner. We're going to find the midpoint, but this time we're going to start the line a little above the F, we're going to drag down and we're going to find the midpoint here on this line, and we're going to work our way over and you can see the heads up display locking is into position, and I'm going to left click and then simply draw the line out to the right, left click again when I'm past the model, and drag it down to somewhere just below the F on this one as well. When you left click, you now have all the section lines that you need, and you can right click and select Continue.
Just like before, you're asked to position the model on the drawing sheet, we can left click, and this time however, you'll notice that the section that you see down here, the hatching, is not included on this side. And if you don't look at drawings like these all the time, it might be hard to recognize. One of the ways I make modifications to my drawings to help people who don't look at this stuff all the time, is to add shading to those section views. If you go to one of those views and hover over until the red dotted line appears, you can right click and select Edit view.
In the dialog box, again you have styles, hidden line, hidden line removed, and you can have one or the other of these, and you can also add shaded to that view. I'm going to go ahead and select OK and you can see here that the shading from the part modeling world has been applied to the drawing as well, it makes it a little bit more clear of how low was cut away and you still have the section lines to help you as well. We're going to to do the same here, we'll right click and select Edit view, and we'll turn on Shaded. Once you click OK, that's updated as well. And with the shading it's much more clear that the bottom section is the actual part and it hasn't been sectioned.
Real quick just as a tip, I also wanted to remind everybody that you could also create projected views from section views, let me show you. If you return to the Create panel and select Projected this time, and instead hover over this view on the right and left click, you can create an isometric view of that section. I'm going to go ahead and left click to place the view, right click and select Create, and you can see that I have my shaded view in an isometric mode now. It's a little off the screen so I'm going to go ahead and hover over my base view on the left.
Left click and drag it down a bit, and then I'm going to left click and drag this view over and here you can see it's still a little bit big, but if we zoom in a bit, let's go ahead and right click on this view, select Edit. You can always change the scale, but again, since we started from a base view, in this dialog box under the scale section, there's a checkmark that says Scale from base. What Inventor's doing by default is using the same scale that you used on the base view, here in this projected view. To change that, you can uncheck this box and then you have the ability to set the scale independently from the base.
For example if we dropped the two to one, and select OK, that shrinks the view just enough so that it fits on the page clearly, and if we zoom in, I think that would help people with the section view quite a bit if they were able to see it like this.
- Reviewing interface changes
- Projecting and importing geometry
- Working with Autodesk AnyCAD
- Understanding part modeling
- Building parts with placed features
- Working with partial chamfers