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Dimensioning a part

From: Up and Running with Autodesk Inventor

Video: Dimensioning a part

In the previous movie, we learned how to draw with the Line tool. During that movie, we created the sketch that you see on the screen, and we are now ready to add dimensions to define the overall size. To begin, we need to get into the sketch environment, and we can do that by double-clicking the sketch in the browser to edit that sketch. You will notice that the Sketch tab is displayed, and we are now in the editing environment, and we are ready to add our dimensions. Inventor only has a single dimension command. It can be found on the Sketch tab under the Constrain panel or through right-clicking to bring up the Marking menu, and selecting the lower-left position.

Dimensioning a part

In the previous movie, we learned how to draw with the Line tool. During that movie, we created the sketch that you see on the screen, and we are now ready to add dimensions to define the overall size. To begin, we need to get into the sketch environment, and we can do that by double-clicking the sketch in the browser to edit that sketch. You will notice that the Sketch tab is displayed, and we are now in the editing environment, and we are ready to add our dimensions. Inventor only has a single dimension command. It can be found on the Sketch tab under the Constrain panel or through right-clicking to bring up the Marking menu, and selecting the lower-left position.

We know that the plate on the screen needs to be perfectly square. So we need an overall height dimension. There is a couple of ways to add this. I am going to show you both ways because both are valid, and depending on the type of sketch geometry you've created, you may select one over the other. While into the Dimension command, we'll start by switching the bottom horizontal line followed by the top horizontal line. We can move our cursor off to the left to where we want our dimension placed, and we can left-click again to place that dimension. After placing the dimension, an Edit dialog pops up, and allows you to enter an exact value for this piece of geometry.

You can now see that the dimension has been placed, the geometry has changed color to indicate that it's fully constrained or dimensioned, and we could move forward. I am going to go ahead and undo this using Ctrl+Z on my keyboard, and show you another way. The first one, I selected two different pieces of geometry. This time, I'm going to enter the Dimension command, and select just the single vertical line. Then when I move my cursor to the left, I get the same dimension I had last time but I had fewer clicks to do it.

Placing that dimension again, I can enter the 1.575 value and hit Enter, and essentially have created an identical dimension. So, either way is completely valid. The reason you would choose one over the other would be in a case where you don't have a single vertical line defining the height. For example, if I were to create two different rectangles here, maybe I am making an L bracket of some sort, and now I enter the Dimension command. There's no single line or piece of geometry that defines the overall height.

In that case, selecting the bottom horizontal line and top horizontal line is the only way to create the overall dimension of this geometry. So, depending on the type of sketch you're creating, either is completely valid and they create identical sketches. It's just a matter of you selecting the one that you need for your design. I am going to get out of the Dimension command by hitting Escape on the keyboard. I am going to delete this geometry because we don't need it. I just wanted to show you a sample of where you could use both types of dimension. We are now ready to dimension our overhang.

The overhang is found on the right, and you can see it because it's the only item that's still green, meaning it's still unconstrained. We are going to start by adding a dimension to locate the top of the overhang. I am going to start by selecting the top horizontal line because that's what I want the base dimension to start from. Now, rather than selecting the line, I can hover over and select the vertex where it meets the square. I can then place my dimension just like I did in the previous dimension, left-click to place that on the screen, and enter a value of 0.212.

Hitting Enter on the keyboard accepts that value, and we're ready to continue on. We're still in the Dimension command, and I need to dimension the position of this overhang at the corner. So, I am going to go ahead and select the top horizontal line again, and this vertex at the corner. Again, I'll place my dimension, and in this case, I am going to enter 0.404. Now, we are almost finished dimensioning the sketch. But the next dimension we need is an angle dimension. As I mentioned, Inventor only has one Dimension command. I want to dimension the angle between this line, and this line.

To do so, I simply select each of the lines, and you will notice after I select the first line, if I hover near the second line, an icon pops up near the cursor, indicating an angle dimension is going to be applied. Simply left-clicking again, and moving my cursor to where I would want to place the dimension, you will notice that I've created an angle dimension. Now, before I place this, I am going to move my cursor to a few different locations. You'll notice that based on where my cursor is the dimension value will change to indicate the angle of the two lines at that location.

Once I find the specific dimension I want to place, I can move my cursor to where I want to place the dimension and enter a value. The final dimension we need to create is very similar to the previous few that we've created, we want to measure the overall distance from the far-left side of the square to the vertex on the corner of the outcrop. I am going to go ahead and place that up near the top of the screen, and enter 1.88 for that value. At this point, we've completely dimensioned our sketch. You can tell that because all the geometry is the darker of the two colors that I have in my color scheme, in this case, purple.

And we are now ready to finish the sketch and begin part modeling.

Show transcript

This video is part of

Image for Up and Running with Autodesk Inventor
Up and Running with Autodesk Inventor

40 video lessons · 8617 viewers

John Helfen
Author

 
Expand all | Collapse all
  1. 1m 28s
    1. Welcome
      41s
    2. Using the exercise files
      47s
  2. 8m 3s
    1. Exploring major workflow steps
      2m 19s
    2. Reviewing different file types
      4m 43s
    3. Exploring essential settings
      1m 1s
  3. 21m 39s
    1. Navigating using the ViewCube
      3m 26s
    2. Navigating using the navigation tools
      5m 36s
    3. Using the browser
      3m 17s
    4. Using the ribbon bar
      2m 10s
    5. Using the Quick Access Toolbar
      1m 4s
    6. Customizing the toolbars
      3m 7s
    7. Using the Marking menu
      2m 59s
  4. 48m 42s
    1. Introducing sketching
      3m 18s
    2. Working with origin geometry
      3m 47s
    3. Understanding constraints
      8m 43s
    4. Drawing with the Line tool
      8m 8s
    5. Dimensioning a part
      5m 0s
    6. Creating parameters
      8m 50s
    7. Creating circles and rectangles
      10m 56s
  5. 38m 31s
    1. Introducing part modeling
      2m 34s
    2. Creating a base extrusion
      5m 12s
    3. Creating multiple extrusions
      7m 35s
    4. Creating a cone by revolving
      6m 12s
    5. Creating holes
      6m 12s
    6. Creating a threaded hole
      3m 3s
    7. Using placed features
      2m 33s
    8. Editing part features
      5m 10s
  6. 25m 52s
    1. Introducing assemblies
      54s
    2. Placing components
      6m 29s
    3. Creating and managing constraints
      7m 50s
    4. Assembling parts
      7m 16s
    5. Understanding the Insert constraint
      3m 23s
  7. 25m 12s
    1. Exploring initial drawing creation
      4m 43s
    2. Placing views
      6m 11s
    3. Creating section and detail views
      5m 10s
    4. Setting basic dimensions
      2m 43s
    5. Changing dimension precision
      1m 24s
    6. Creating baseline dimensions
      1m 52s
    7. Creating center lines, center marks, and hole notes
      3m 9s
  8. 1m 20s
    1. Next steps
      1m 20s

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