# Dimensioning

## Video: Dimensioning

Dimensioning is one of the primary ways you can add intelligence to a sketch. We've been creating sketch geometry and you've probably I now have a blank part file. And selecting one of the planes in the origin geometry.

## Dimensioning

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.

Show transcript

#### This video is part of

Inventor 2014 Essential Training

90 video lessons · 3326 viewers

Author

Expand all | Collapse all
1. ### Introduction

1m 24s
1. Welcome
47s
2. Using the exercise files
37s
2. ### 1. Basic Concepts

6m 20s
1. Exploring major workflow steps
2m 19s
2. Reviewing different file types
4m 1s
3. ### 2. Navigating the Interface

22m 3s
1. Navigating using the ViewCube
4m 56s
2. Navigating using the navigation tools
5m 31s
3. Using the browser
3m 34s
4. Using the ribbon bar
2m 47s
42s
4m 33s

22m 6s
6m 40s
2. Custom ribbon bar panels
6m 22s
3. Keyboard
5m 9s
3m 55s
5. ### 4. Leveraging the Project

20m 24s
1. Project file introduction
3m 54s
2. The project file: .ipj
4m 4s
3. Setting up the project file for this course
7m 11s
4. Frequently used subfolders
5m 15s
6. ### 5. Sketching Concepts and Settings

22m 31s
1. Introducing sketching
4m 55s
2. Working with origin geometry
4m 46s
3. Understanding constraints
7m 39s
4. Application options
5m 11s
7. ### 6. Creating Geometry with the Draw panel

50m 43s
1. Drawing lines
6m 29s
2. Creating rectangles and arcs
9m 26s
3. Creating splines
6m 35s
4. Creating slots
5m 43s
5. Construction geometry
6m 18s
6. Dimensioning
9m 34s
7. Parameters
6m 38s
8. ### 7. Editing and Modifying Sketch Geometry

30m 33s
1. Move, copy, and rotate sketch geometry
7m 43s
2. Trim, extend, and split sketch geometry
6m 20s
3. Scale, stretch, and offset geometry
7m 47s
4. Creating rectangular, circular, and mirrored sketch patterns
8m 43s
9. ### 8. Work Features

19m 27s
1. Understanding work features
3m 58s
2. Creating offset work planes
4m 17s
3. Creating work planes
6m 59s
4. Creating work axes and points
4m 13s
10. ### 9. Projecting and Importing Geometry

16m 50s
1. Projecting geometry
7m 7s
9m 43s
11. ### 10. Understanding Sketch Feature Creation

54m 31s
1. Part feature introduction
5m 14s
2. Creating a base extrusion feature
8m 46s
3. Keeping extrusions connected with the To next face/body option
4m 29s
4. Creating revolves
7m 42s
5. Creating complex shapes with the Loft tool
8m 50s
6. Adding control to a loft by creating rails
8m 40s
7. Creating a sweep feature
6m 16s
8. Creating a sweep feature with model edges
4m 34s
12. ### 11. Building Parts with Placed Features

24m 44s
1. Adding holes to a part model
10m 10s
2. Modifying edges with fillets and chamfers
4m 18s
3. Hollowing parts with the shell feature
10m 16s
13. ### 12. Creating Patterns of Features

25m 37s
1. Creating rectangular feature patterns
9m 23s
2. Adding intelligence to a rectangular pattern
5m 45s
3. Creating rectangular feature patterns along a path
2m 22s
4. Creating circular feature patterns
3m 11s
5. Mirroring part features
4m 56s
14. ### 13. Creating Configurable iParts and iFeatures

31m 30s
1. Understanding iParts and iFeatures
3m 19s
2. Creating an iPart from an existing part
11m 0s
3. Changing between versions inside an iPart
5m 50s
4. Extracting iFeatures for use in other parts
5m 11s
5. Inserting iFeatures into a part
6m 10s
15. ### 14. Adding Parts to an Assembly File

26m 23s
1. Introduction to assemblies
1m 59s
2. Placing components
7m 40s
3. Creating components in the context of an assembly
8m 9s
4. Placing fasteners from the Content Center
8m 35s
16. ### 15. Using Constraints to Position Parts

46m 14s
1. The Mate/Flush constraint
9m 42s
2. The Angle constraint
5m 34s
3. The Insert constraint
3m 55s
4. Driving constraints
10m 0s
5. The Transitional tab
3m 50s
6. The Motion tab
9m 18s
7. Contact sets
3m 55s
17. ### 16. Assembly-Visualization Techniques

18m 38s
1. Adding materials to parts in an assembly
4m 3s
2. Visual styles
4m 52s
3. Enhancing the design experience with shadows
2m 9s
4. Adding a ground plane, reflections, and perspective to a design
3m 34s
5. Changing the lighting style to match a design
4m 0s
18. ### 17. Creating Drawing Views

39m 11s
1. Exploring initial drawing creation
5m 6s
2. Placing base and projected views
9m 31s
3. Creating section views
8m 0s
4. Creating detail views
3m 56s
5. Creating a breakout view
5m 41s
6. Creating auxiliary and cropped views
6m 57s
19. ### 18. Setting Basic Dimensions

25m 57s
1. Creating general dimensions
9m 20s
2. Changing dimension precision
4m 21s
3. Creating baseline, ordinate, and chain dimensions
5m 51s
4. Creating baseline, ordinate, and chain dimension sets
6m 25s
20. ### 19. Creating Balloons and a Parts List

10m 43s
1. Creating individual balloons
4m 34s
2. Creating a group of balloons with automatic ballooning
3m 40s
3. Adding a parts list to the drawing
2m 29s
21. ### Conclusion

30s
1. Next steps
30s

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