Join John Helfen for an in-depth discussion in this video Placing views base and projected views, part of Autodesk Inventor 2018 Essential Training.
- [Voiceover] Now that you can create drawing sheets, let's look at how we can create drawing views to be placed on those sheets. Go ahead and start a new drawing, and when your drawing sheet is created, we can begin placing views onto the sheet, and there's a couple ways to do that. We can either go to the Place Views tab in the Create panel and select Base, or we can right-click in the Graphics window and select Base from the Marking menu. Once we do that, you'll get a Drawing View dialog box, and it has basic information that we're going to use to create these drawing views. Right now, we don't have any files open.
If we did, there would be files listed in this drop-down right here on the dialog box. Since we don't, let's go ahead and use the Browse button on the right-hand side, and this will open up a File dialog window where you can browse to the file you want. I've selected Engine Block as my part file. You can scroll down and find it, and then simply click Open. By doing that, you've told Inventor that's the part you want to use to create drawing views. You can also see that the file is listed here in the drop-down now. Just below that is the Representation.
Every file is going to have a master Representation. If you have additional Representations, you can select from them here in this list. You might have a Representation that shows an assembly with no standard parts, or you might show it with parts in different positions. In this case, we're going to leave the default, and we'll look at the section to the right, Here you can see we have different styles that are available. We have Hidden Line, we have Hidden Line Removed, and we have Shaded. This will allow you to make different configurations of the visual style of this specific drawing view.
We'll go ahead and leave the default. Below that, we have the View Label, which you can change if you need to, but I typically just leave the defaults. And then, below that, we finally have Scale. This view, that you see on the screen, is a little bit small, so let's go ahead and change its scale. Let's bump it up to 2:1. If you wanted to, you could continue going as large as you needed, and you can always make edits and return to a different scale at any point. I'm going to go ahead and set to 2.1, and now we can look at what's going on in the Graphics window itself. If we hover over this view, you'll notice that we can left-click and drag it and place it anywhere on this drawing sheet.
I'm going to go ahead and find a location right here near the middle at the bottom, and I'm going to release my mouse button. Now what I'll do is, as I move my cursor, you'll notice that Inventor is automatically projecting additional views for us, based on that base view. If, for some reason, the view is not in the proper orientation, that's what this View Cube is for. Unlike in the Part Modeling and Assembly Modeling environment, where this would rotate your entire viewpoint in the Graphics window, here, in the Drawing View, it's going to rotate this view in that View.
So, for example, if I didn't want to look at it from this location, I could simply use my standard functions on the View Cube to rotate the orientation. It works just like the View Cube does in the Modeling Environment, but it's changing the orientation of this specific view. You can even switch to an isometric view if you want. I'm going to go ahead and return to the front view, and I'm going to left-click just to the left of that model, I'm going to left-click upwards and to the left, and I could continue around and generate views in any position I want.
The other way I could do it is, in this base view, you can see arrows in all those directions as well. Simply clicking on those will toss a view out onto the paper, and you can work your way around and create all the views you need. Now that we have all the views created, I wanted to mention that you can also change your orientation of your view at this point as well. The difference is is rather than just changing one view, you're going to change all the views based on that. Now, you're probably going to set your orientation before you start this, but just in case you make a mistake or find that, when you're laying out drawing views, a better orientation would be more proper, you can make these changes right here.
Once you have your views in the position that you want, you can right-click and select OK. What that does is it allows Inventor to quickly create your drawing views, it just took a couple of seconds and we got all our drawing views, and just like the Part Modeling and Assembly Modeling environments, the Browser and the Graphics window are perfectly linked. The Browser is essentially just a new lens into what's on the Graphics screen. Let's take a look. If we have a look over in the Browser, you can see view one, EngineBlock.ipt, and when we select it, it highlights in the Graphics window.
Below that are the nested projected views. Here's the one on the left, here's the one at the top, and here's the one at the right. These are all nested because they're linked to the base view. Below that, we have the isometric views, the one in the upper left and the one in the upper right. What's important about these is they're not nested under this EngineBlock.ipt, because they can be moved anywhere and they're not aligned to that base view. Let me show you what I mean. If you hover over that view, and wait for the red dotted line to appear, you can left-click on it and drag, and reposition this isometric view anywhere you want on the page.
The same is not true for the other projected views. If we hover over the view on the left here, and left-click and drag on its red dotted line, you'll notice that an alignment line connects it to its base view. I can move my cursor up and down, but the only movement I can make of this view is to the right and left, because it's trying to maintain the alignment. The same is true for the view at the top. If you left-click and drag on its red dotted line, it's aligned vertically. Before we finish up, I want to mention that, if for some reason you find that you've missed a view, or you've made a mistake and maybe deleted a view-- If we right-click on this view and select delete, you can remove a view from the sheet.
It also gets removed from the Browser. But, if you need to recreate or add an additional projected view, that can also be done, and you're going to need at least one other view on the page, which we have, in order to create the projected view. To do that, we need to return to the Create Panel on the Ribbon Bar, and this time select Projected. What Inventor's going to want is you to select a view that it can use as the base view, and it simply places you back into the Projected View mode that we saw when we were creating these views in the first place.
If you left-click to locate it, then right-click and select Create, Inventor will recreate that view for you, you can see it's here in the Browser again, and it's been linked to that base view, so it has proper alignment.
- Reviewing interface changes
- Projecting and importing geometry
- Working with Autodesk AnyCAD
- Understanding part modeling
- Building parts with placed features
- Working with partial chamfers