# Adding and removing relationships and dimensions

## Video: Adding and removing relationships and dimensions

Relationships and dimensions are what take simple sketch entities

## Adding and removing relationships and dimensions

Relationships and dimensions are what take simple sketch entities and define it into the design you're working on. Relations can control size, location, and equality between sketch elements. And dimension can control angles, physical shape, and the distance between elements or the origin. Let's take a look. I have a sketch open on the top plane. And I have a few different examples here laid out on the screen. First things first, let's take a look at the two lines over here. So I click on the first line here. As soon as I let go of the left mouse button I get a couple options. And notice these are context sensitive.

I only have one line selected, so I only have two options. One I can make it horizontal, or two I can make it vertical. And then finally I can make it fix, and fix just means if I click on it, it just can't move anywhere, it's just stuck where it is. So I don't normally want to use that one, so turn that off. And notice how I did that, and how I got deleted that? Go back, just click on the green box and hit Delete on your keyboard, or you can right-click on the green box. And choose Delete from the Menu. Next if I choose two lines, this line here, hold on Ctrl, slip the next line, next door to it. I've got a lot more options.

So I can say these lines are horizontal, they're vertical, they're co-linear, they're perpendicular, they're parallel, or they're equal. In this case, let's try out parallel. Wherever they are, they happen to be parallel. And if I grab one, I can move it around. Notice they operate as a team now. They're both parallel no matter where they are. And I can move things around, I can still change the length. If I want to make them the same length, I could also add a secondary relationship. Choose both of the lines by holding down Ctrl, and I'll say Equal. Now they're parallel and they're equal. Notice now they are not spinning around. But what I can do is, I can use that little fix icon.

So click on the tip, not the whole line itself, but one of the points on either end, and choose Fixed. Now I have a fixed dimension. If that point doesn't move, then these points here will move around. So it makes it so it could actually simulate some motion inside of my sketch and see how things actually work and layout. Down here, I can choose these lines here. Choose both of those lines. I can say these lines are for instance co-linear. And then put them on top of each other. I can drag it out. And you can still see the point here. And they can be separate lines, or they can be on top of each other. As long as they're co-linear, they all operate as a team.

And there's this little dashed line showing that those two lines are co-linear. In fact, you can even bring this point, and drop it on top of that point there, and that adds a coincident relationship. And now those two points, it's two separate lines, but they're still connected together in a co-linear fashion. Up here you got a couple of circles. Go ahead and choose both the circles by holding Ctrl. As soon as I let go of those circles, I could say these circles are co-radial, or they're tangent to each other, or they're concentric. Let's try all three. First one, co-radial. That just puts them exactly the same as one circle on top of the other, which is really not what we probably want to do in this case, but it does put those two circles exactly on top of each other.

Hit Undo to bring it back. Choose them both again. This time, I'm going to say, these are tangent, so that means they're touching each other. And I can roll this thing around. It maintains a tangency. And, it's a nice way to add the tangency. If you don't like it, you can always delete the tangency. Hit Delete on your keyboard, take it off, now you can move it back away. Select them both again. This time, choose Concentric. Now you have one circle inside the other one. And wherever they move, they'll move as a team. You can adjust different things here. And when you have a couple of circles like this. When we add dimensions, you can add a dimension by choosing the inside circle and placing a dimension, maybe 1 inch.

You can also dimension from the inside circle to the outside circle. Maybe a quarter inch. And I'm adding those dimensions by clicking in the first circle, then choosing the second circle, and then finally, choosing where I would like to place the dimension. And notice, I already have the dimension placed. So if I choose this one, it's going to say, hey, you're doing something wrong here. Notice everything turns yellow, and you're saying, hey. You've already placed a dimension on that sketch. And you'll already defined it as a quarter of an inch. Do you want to add it again? So it's asking you a question. Make this dimension driven? Driven just means, it's just a reference dimension. It doesn't actually control the design.

Or you can maintain it driving dimension, and it'll actually cause an error in the sketch. So I make it driven. Notice it turns grey, and the other ones turn black. So if I change the dimension here to become 0.375, it automatically updates as well, because it's just a reference dimension. However, if I were to go back and add a dimension from here to here. And I said, hey, I actually want to make this a driving dimension, click OK. Now, what happens is, this whole thing says, it's unsolvable, because it doesn't know, is it use, supposed to use this dimension here. Or this dimension here, because it's giving the same information, by both of them.

So what you can do is delete either one of them. And then it's back to being happy. Notice all the lines are still blue, though, because they don't know where they are. So to solve that problem, we either need to place this on the origin, or add a relationship to where it is in space. One of the great ways to do that is using the Center Line tool. So, I'm going to make a line from here and bring it right up to the top. And now wherever I drag this thing, I've got a couple of lines that attach me to the origin. You can add a dimension by clicking the line, I'll say 0.75. And, over here, I'll say this is going to be 2.5. Notice as soon as I do that, everything turns black and it knows exactly where it is, because we always want to relate our sketches to the origin.

So they know where they are in space. Continuing on, let's go ahead and grab the Smart Dimension tool. And here's an angle. I want to define the angle. To do that, you're just going to choose the first line And then again choose the second line. And then you're going to place the dimension. However dimension tool is dependent upon where you place it in relationship to the angle. So over here, I've got 30 degrees or 30.96 degrees. As I move this around the circle notice that it's the same angle, it's just showing you how it would place the dimension differently. Same thing over here. Same thing down here. So as you move around that circle, it keeps changing, how it's going to place the dimension.

In this case here I just want to place it inside. I'll type in 30. Click OK and adjust the dimension. These lines can still move, but it is now defined as 30 degrees. So I can't change the angle. I can still just move things around. So again I'd want to tie that into the origin or tie that into something else. And finally, I've got this rectangle here, and I want to add a few dimesions to that. To do so, I'm going to go ahead and choose the Dimensioning tool. There's a couple of different ways to use the Dimensioning tool. Number one is, I could just choose a line itself and put a dimension. Which is fine, however, what happens if it was not a full line? What if that line didn't continue the full length? For instance, I'm going to give you a sneak preview here on the Sketch Fill It tool, and I'm going to fill these corners.

They're going to have a rounded corner to those four corners. Okay, I'm going to increase the size. Now, in this case here, if I use a Smart Dimension tool, it only dimensions that length. So, I'll take 2.0, its only dimension from here to here. It's not the full length of the shape. It's really not what I want. So go ahead and delete that. Grab the Dimensioning tool. This time, I'm going to dimension from the left-hand side all the way over to the right-hand side, and then third, I'm going to place the dimension. That's called a 3 pick dimension. I can type in, 2.5 and place the dimension. I always try to use a 3 click dimension because it allows me to radius the corners or make other changes, and it doesn't affect that filed dimension.

Adding and using relations can be a huge time saver and makes your sketches easier to update and simpler to understand. Relationships and dimensions are used throughout Solidworks. And an understanding of how they work is extremely important.

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#### This video is part of

SolidWorks 2014 Essential Training

97 video lessons · 7149 viewers

Author

Expand all | Collapse all
1. ### Introduction

1m 51s
1. Welcome
1m 7s
2. Using the exercise files
44s
2. ### 1. Touring the Interface

31m 13s
1. Launching SolidWorks for the first time
3m 55s
2. Accessing and customizing the Ribbon
4m 14s
3. Touring the shortcut bar and identifying essential keys
7m 27s
4. Saving, renaming, and managing files
10m 28s
5. Working with the new view cube, or View Selector
2m 36s
6. New features in SolidWorks 2013 and 2014
2m 33s
3. ### 2. Getting Started with 3D

14m 11s
1. Understanding the 3D world
2m 31s
3m 15s
3. The virtual, parametric prototyping environment
1m 56s
4. The FeatureManager and feature-based modeling
3m 43s
5. History-based modeling and the rollback bar
2m 46s
4. ### 3. Basic Solid Modeling

28m 32s
1. Starting a new sketch
6m 50s
2. The six steps used in almost all modeling features
52s
3. The Line and Centerline tools
3m 25s
4. Using the Circle tool
1m 51s
5. Adding and removing relationships and dimensions
6m 56s
6. Understanding relationship types
3m 58s
7. System options, units, and templates
4m 40s
5. ### 4. More Drawing Tools

18m 28s
1. Drawing rectangles
5m 31s
2. Creating arcs in a sketch
4m 8s
3. Drawing splines in a sketch
4m 57s
4. Sketching polygons
3m 52s
6. ### 5. Sketch Editing Tools

36m 5s
1. Trimming and extending portions of a sketch
3m 54s
2. Creating offset geometry
3m 13s
3. Moving, copying, rotating, and scaling elements
3m 13s
4. Erasing, undoing, and redoing actions
2m 24s
5. Using the mirror tools
2m 24s
6. Creating repeating patterns in a sketch
4m 55s
7. Using construction lines to build robust sketches
3m 25s
8. Applying fillets and chamfers to a sketch
2m 32s
9. Working with slots
3m 46s
4m 1s
11. Using the Convert Entities command
2m 18s
7. ### 6. Reference Geometry

9m 33s
1. Working with planes
5m 28s
2. Placing and using axes
2m 22s
3. Placing a coordinate system
1m 43s
8. ### 7. Building 3D Geometry

17m 50s
1. Extruding a sketch into a 3D object
4m 36s
2. Using Revolve to create 3D parts
2m 42s
3. Using Loft to create complex shapes
4m 40s
4. Refining a loft shape with guide curves
2m 22s
5. Using the sweep to create wire and pipe shapes
3m 30s
9. ### 8. Removing Material

20m 23s
1. Modifying parts using the Extruded Cut tool
5m 42s
2. Working with the Revolved Cut tool
6m 19s
3. Using the Lofted Cut tool
3m 32s
4. Cutting holes and grooves with the Swept Cut tool
4m 50s
10. ### 9. Refining Geometry

21m 5s
1. Using fillets and chamfers to smooth corners
5m 58s
2. Creating repeating rectangular patterns
3m 16s
3. Creating a circular pattern
2m 27s
4. Mirroring objects
4m 0s
5. Using the Shell and Draft tools
3m 52s
6. Scaling parts
1m 32s
11. ### 10. Blocks

9m 39s
1. Working with reusable sketches and blocks
2m 47s
2. Creating blocks
3m 51s
3. Designing with blocks
3m 1s
12. ### 11. Assembly: Putting It All Together

29m 45s
1. Understanding the tools for beginning a new assembly
4m 46s
2. The basic steps in creating an assembly
3m 18s
3. Mating parts together in an assembly
6m 43s
4. Working with subassemblies
2m 9s
5. Linear and circular assembly patterns
4m 56s
3m 32s
7. Using Toolbox
4m 21s

15m 8s
1. Mating parts with coincident, parallel, and distance mates
4m 35s
2. Mating parts with width mates
5m 53s
3. Mating parts with path mates
2m 5s
4. Mating parts by aligning planes
2m 35s
14. ### 13. Hole Wizard

10m 20s
1. Getting started with the Hole Wizard
4m 38s
2. Positioning holes in layout sketches
5m 42s
15. ### 14. In-Context Modeling

15m 27s
1. Linking sketches to other parts
4m 28s
6m 48s
3. Using the Hole Wizard in context
4m 11s
16. ### 15. Creating Threads on Parts

17m 15s
7m 17s
2. Using a helix and Swept Path to create a thread
4m 2s
5m 56s
17. ### 16. Equations and Design Tables

17m 25s
1. Using equations to drive a sketch
5m 5s
2. Working with complex calculations
2m 6s
3. Integrating Microsoft Excel to manage design tables
7m 10s
4. Building assemblies using part configurations
3m 4s
18. ### 17. Part Drawings

23m 17s
1. Working with drawing templates
6m 49s
2. Setting up drawing options and sheet properties
3m 43s
3. Choosing the correct projection angle
2m 21s
4. Adding model views to a drawing
10m 24s
19. ### 18. Dimensioning

16m 8s
1. Creating general dimension notations
6m 37s
2. Creating ordinate and running dimensions
3m 0s
3. Dimensioning holes and curved features
3m 8s
4. Using the autodimension tools
3m 23s
20. ### 19. Adding General Annotations

14m 38s
1. Creating holes and callouts
5m 8s
2. Adding center marks and centerlines to a drawing
3m 46s
2m 57s
4. Making drawing revisions
2m 47s
21. ### 20. Assembly Drawings

11m 42s
2m 10s
2. Including a bill of materials
1m 42s
3. Adding balloons to specify parts on an assembly drawing
1m 39s
4. Adding a title block and sheet properties
2m 8s
5. Building an exploded view for an assembly drawing
4m 3s
22. ### Conclusion

1m 2s
1. Next steps
1m 2s

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