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Dimensioning is one of the primary ways you can add intelligence to a sketch. We've been creating sketch geometry and you've probably seen some dimension show up in the heads-up display. But I want to walk through it a little more clearly and explain a few of the options you have. I'm going to start a new Part file by clicking New on the tool bar, selecting standard.ipt and then clicking Create. I now have a blank part file. I'm going to create a sketch by clicking create 2D sketch. And selecting one of the planes in the origin geometry. I'm now in the sketch environment and can begin showing you how to create dimensions.
I'm going to start with the most simple type of dimension. And that's what you may use while dimensioning a single line. Now as I create this line you'll notice the heads up display is showing me a dimension. It's actually showing me two. It's showing me the over all length of the line. And the angle that that line is at compared to horizontal. So if I wanted to create the dimension while creating the sketch geometry. I can simply type 1 on my keyboard. Hit Tab to switch to my angle dimension. And you can now see if I move my cursor, the line stays at a 1" length.
The heads up display shows a lock next to it, indicating that I've entered a value. And I can now enter a value for my angle dimension. Now, I don't have to do it, but, if I want to, I can type four, five, hit tab on my keyboard. And you'll see that I now have a line, 1" long, at a 45 degree angle. The only other thing remaining is to locate that endpoint by left clicking. By doing this, you've, you can see that during sketch creation the heads up display allows me to create dimensions on the fly.
I'm going to go ahead and undo this, by right-clicking and selecting Undo. And I'm going to get back into the Line command and show you how to manually create these dimensions. I'm going to start with a basic line. In this case, rather than enter a value for the heads up display, I'm going to just use it as a reference. This allows me to draw roughly to scale. I know that this is 0.96. Now it's just over one inch. And that's close enough for my quick sketch. I don't need it to be exact. I'll go back and add dimensions later. Next, I'm going to go ahead and create a line at off at some angle.
I'm going to right-click and select OK to get out of the command. And I'm now ready to right-click and select General Dimension. If I hit Escape on the keyboard, I could also get to the Dimension command from the Constrain panel here in the Sketch tab. But, again, I prefer the right-click method. Especially, within Sketching because I do a lot of sketching of geometry and creation of dimensions. It just saves some of my mouse travel. Now that I've created this geometry, I have a few different ways to dimension it. I can select the end points of these lines to dimension the overall length.
And while that's perfectly acceptable, I can left-click and place this dimension. And I can even hit 1 and Enter, to give it a specific length. Now in that step I had to select two separate points to create this dimension. I'm going to go ahead and right-click and, and cancel out of this command. Right-click again and select Undo, to get out of the dimension, I just created. Now I'm going to get back into the Dimension command and show you another way you can do that. Rather than selecting the end points, I could simply select the line itself.
Now, it might not seem that important, but overall when you're sketching, saving one-click for every dimension is going to add up over time. So, it's just a matter of finding that method that works for you, and is most efficient while you're designing. Either of them is perfectly acceptable. But, I think, over time, you'll find selecting the lines a little bit easier to do. I'm going to go ahead and locate that dimension, and enter one again. And you can see that my line is updated. Now I'm still in the Dimension command, but in this case I'm going to go ahead and select that line one more time.
And it looks as if I'm going to create that same dimension again. Now instead I'm going to hover over this angled line and you'll notice that I get a heads up display indicating an angle dimension. While inventor only has one dimension command it has the capability of creating all the dimensions you're going to need while designing. If I left-click to select that line, you can now see I'm creating an angle dimension. If I move my cursor around to place the dimension. You'll also notice as I move across the line, it will change the location of the dimension and its value based on where you're locating your cursor.
So it's important to know where you're placing the dimension And that you can change that on the fly very easily so that you get exactly the dimensions you need. If I left-click again and enter 45, I now have an angle dimension for 45 degrees. Now, there's one more dimension missing here. And, it's the length of this overall line. And there's a couple of ways we can get to this. If I select this line first, and move my cursor, out past the edge of the geometry.
You can notice that I can create a horizontal dimension or a vertical dimension. Either one, doesn't matter. It is a way to dimension this line. Now, there's one other way we can dimension this. While I'm moving my cursor, if I right-click, I do have the option for Horizontal, Vertical, or Align. I can easily get to Vertical or Horizontal, as you just saw, by moving my cursor. Align, however, has to be selected from this menu. If I select Aligned, I now have the actual length of that line, rather than its dimension relative to the original horizontal line at the bottom.
If I placed that dimension, I can enter 1, hit Enter. And I now have both of these lines at 1" long, at a 45 degree angle from each other. Next, I'm going to show how to create dimensions for circles. I'm going to right-click and instead of hitting OK or getting out of this command, I'm going to jump right to the circle command. I'm going to left-click to locate my center point, and you can see I get a heads up display for this geometry as well. Just like the line, I could enter my value here and have it automatically create the dimension.
But I want to show you how to convert between creating diameter and radial dimensions. So, I'm simply going to left-click to pick a random size for this circle. And I can now, right-click and get back into the Dimension command and select the line to create that dimension. Let me hit Escape one more time real quick, and do that one more time. Because you'll notice, just like when we were going the angle line over here. When I hover over the circle, you'll see that I get a diameter dimension, or a diameter icon. By left clicking and moving my cursor, you can see I'm going to add a diameter dimension.
Now, just like when we were creating the Horizontal, Vertical and Aligned dimensions. Even if while you're still waiting to place this dimension or locate it, you can right-click and you have dimension types of Radius and Diameter. Selecting either one will toggle back and forth. While you're still locating the dimension you can toggle back and forth as many times as you want. And Inventor will actually remember the last one you use. So if you generally do radius dimensions or diameter dimensions once you've converted to it, it's going to remember that from that point forward.
I'll go ahead and place this dimension, hit 0.5 as my value, and when I hit Enter, I now have that diameter dimension located. The final item I want to show is how to use multiple pieces of geometry in dimension across them. I'm going to create a very simple shape. I'm going to create two different rectangles. And then the sizes don't really matter here, I just want to point out a couple important items. First, as I, create a second rectangle on top, what you'll notice here is I don't have a single solid line that represents the overall height.
Now I have a single line over here to define the height of this rectangle, and a line here, to define the top rectangle. But I can't select a single line that defines the overall length. If I get into my Dimension command, you can see I do have a single line for the overall width of the part. But from a height standpoint, I can't get the overall height. So I could go back to what we talked about in the very beginning and select the endpoints of this overall height to get its dimension.
I can also select this top line, and it looks like I'm going to dimension the overall width. But if I hover down over the line at the bottom, you'll notice that I have the overall height. Now what it's essentially done is selected the endpoints for me automatically. But, it's a way to use the overall lines as a bigger target for selecting dimensions. It sounds really silly, but over time, selecting those individual endpoints can get a little bit tedious. And I find that the overall length of the line is a little easier target to hit and it makes my design a little bit faster.
I think as you get into sketching a little more, I think you'll find these tips helpful.
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