Join John Helfen for an in-depth discussion in this video Create general dimensions, part of Autodesk Inventor 2018 Essential Training.
- [Voiceover] Now that you understand how to create drawing sheets and drawing views, let's take a moment to look at how we can begin adding dimensions to our drawings. On the screen I have an engine block dimensions drawing that we're going to use for this exercise. To begin creating dimensions, we need to go to the annotate tab. Within the annotate tab, you have all the things that you're going to need in order to create information on this drawing. Such as dimensions, feature notes, texts, symbols, and other items. Dimensions within drawings work in almost exactly the same fashion as dimensions within a sketch environment, with one minor difference.
In the sketch environment, you're creating dimensions to drive the size of the model. In the drawing, you're actually creating dimensions to provide information about manufacturing. Those types of dimensions are not always going to be the same. The one thing that's different about dimensions in drawings, is that they need to be much more organized. Let's go ahead and start looking at the dimension command, and we'll talk about it as we move along. To begin, we need to go to the annotate tab in the dimension panel, and select dimension. We can also access it by right clicking in the window and selecting general dimension, just like we do in the sketch environment.
Let's go ahead and scroll in on the view on the top here. And we can look at some basic dimension information. Just like in the sketch world, you have the ability to select specific end points or specific lines. For example, if we select the first end point, and then select the second endpoint, we can then place our dimension. But what you'll notice here is, as I used my cursor away from the dimension, it snaps and turns to a dotted format. That indicates that it's positioned at a specific increment. If I move my cursor up a little bit further, you'll see that I snap again.
And that continues to repeat every so often. The reason for this is, it allows you to very easily organize your dimensions. For example, if I left click to place this dimension, it's nice and positioned centered, and it's just a slight distance off the line we just dimensioned. While we're still in the command, let's go ahead and select this larger line just below it. And here you'll see the same. We still have the snaps, and we can overlap geometry. But if we hover over the dimension, the 85, and then drag upwards, you'll see we snap into a nice organized stack of dimensions.
This really helps when you're creating dimensions for a large drawing. And it helps keep everything organized and easily controlled. Next we'll double click the middle mouse button to zoom out. And we're gonna scroll in on the view in the bottom corner. And we'll look at how we can add different types of angled dimensions. While we're still in the dimension command, I'll select the line on the top of the cylinder. And you can see Inventor automatically wants to create a linear dimension. But just like in sketching, if you hover over the line that's on an angle, you get a heads up display that says we're going to create an angle constraint.
Left clicking selects the line. And again, just like in sketch, as you move your cursor, you're going to find that the dimension follows you. And changes and updates based on the position of the cursor. I'm going to go ahead and create the dimension just to the right of the model. And you'll notice that the 15 is below the dimension. I want to go ahead and flip this to the other side. So I'm going to go ahead and right click and select okay to get out of our dimension command. And then I'm going to hover over the 15. And as I left click and drag, you can see I'm placed back into a position where I can start locating this dimension again.
As I hover my cursor into the dimension, you'll see I get a center line. If I move just above that, you'll see that that dimension flips. If I go too far it changes dimension, but I'm going to find that center line. And then simply drag up a little bit and release my cursor to reposition that dimension. Next we'll look at how we can create aligned dimensions. Let's go ahead and right click, and select general dimension. And this time we're going to go ahead and select the angled line here on this top face. If we drag our cursor straight up, we get a linear dimension.
If we drag our cursor straight to the side, we get a linear dimension. If we hover our mouse closer to that line, you'll notice that it becomes aligned. If we were to left click here, we would place an aligned dimension. And then we could simply drag that to reposition it maybe further out here. The other way we can do this is just like in sketches. We can right click while we're in the mode where we can place the dimension, and we have a dimension type fly out that we can select horizontal, vertical, or aligned. By selecting aligned we're forcing Inventor to create an aligned dimension, so that we can position it while we are creating the dimension.
Let's go ahead and zoom out. Double click on your middle mouse button. And then let's go ahead and zoom in on the view on the bottom right. Here we'll go ahead and look at how to create radial and diameter dimensions very quickly. We'll go ahead and select the circle in the center of the view. And as you can see, we default to a diameter dimension. And simply left clicking will place that dimension at that location. While we're still in the dimension command, let's select the circle just to the outside of that. And this time while we're in a position where we can place our dimension, just like for the aligned and just like in sketch, if you right click, you have the ability to change from a diameter to a radius.
Simply left clicking will create the radius dimension for you. Hopefully you can see how similar sketching and drawing dimensions are, but you can understand how the organization tools will help to make very clear drawings.
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