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Creating rectangles and arcs

From: Inventor 2014 Essential Training

Video: Creating rectangles and arcs

As we continue to learn about the drawing tools, I want to use an If we look at this from the front of the model, you We're going to go ahead and start a blank part to create this feature.

Creating rectangles and arcs

As we continue to learn about the drawing tools, I want to use an actual, physical part, so that people understand the context in which we're drawing. In this case, we're going to use this basic computer mouse shape. We won't create the entire thing, but we will create most of the body, so that you can see how sketching works with part modeling, while you're learning about how to create rectangles and arcs. If we look at this from the front of the model, you can see that there's a curvature at the top of the mouse. And if we look at it from at it from the top, you can see that there's curvature on each side of the mouse as well.

We're going to go ahead and start a blank part to create this feature. And walk through the process as we go. I'm going to click on the New button on our Quick Access toolbar, to bring up the create new file dialogue. Next we'll select standard.ipt, and then click Create. This'll create a new blank file that we can start creating our mouse shape in. To start, we need to create an initial sketch, to create our base feature for our part. To do this, we can right-click and select, New Sketch, from the Marking menu or we can select, Create 2D Sketch from the Sketch panel on the 3D Model tab.

For this demonstration, I'm going to mainly stick to the right-click marking menu where appropriate. I'm going to select new sketch which will bring up the origin geometry. And I'll select the x, y plane here in the center, to use as my flat surface to sketch on. We're now ready to create the rectangle that'll define the overall shape of the mouse. From the side view. I'm going to right-click, and select two point rectangle from the marking menu. And then hover near the center point that was projected to the sketch, in order to lock the start point of the rectangle, to the center point of the sketch.

As I hover near that you'll see the green dot pop up, indicating that Inventor is going to apply a coincident constraint. To lock the starting point of the rectangle to the center point. By left-clicking, I can start my rectangle and as I move my mouse, you'll see the heads up display, showing dimensions with values in them. I can either use these dimensions as reference, or I can use the Tab key, to switch between them and actually enter an exact value. In this case, we're going to enter four for the length, and then we're going to hit Tab to move to the height, and we'll enter 1.5 and hit Enter on the keyboard to create the rectangle.

Now, the rectangle is off the screen a bit. We can either click the front view of the view cube, or in this case I'm going to double-click my middle mouse button, which will zoom everything into the graphics windows. Then I'll use my scroll wheel to zoom out just a little further so I can clearly see what I'm working on. I'm going to right click and select Okay to get out of the rectangle command. And we're now ready to create the arc that defines the top surface of the mouse. In the draw panel on the toolbar, I'm going to select three point arc. If you don't see three point arc, you can use the drop down menu to select three point arc from the expanded menu.

Down in the status bar in the bottom left-hand corner, you can see that it's telling me to select the start point of the arc. In this case, I'm going to use the midpoint of this vertical line as my start point. And as I hover near the midpoint, I get a green dot, which indicates Inventor's going to add a coincident constraint. I'm going to left-click to start the arc and the next thing I need to do is select the end point for the arc. And in this case I'm going to select something between the midpoint and the top of the rectangle, somewhere near the top. And I'll left-click to locate the end point and then as I move my cursor you can see that the radius can be defined as concave or convex.

Depending on my needs. In this case, I'm going to ma, hover up near the top of the rectangle and then Invetor's going to snap to that line, and create a tangent constraint for me automatically, which is exactly what I want. I want to make sure that this arc only touches the very top of the rectangle at one point. I'm going to left-click to define that point and my arc is created. I can then right-click and select Okay to get out of the command. And if you want, depending on where you've selected, you can make adjustments at this point. I'm going to left-click and drag the endpoint of the arch.

And I, you, you can see that the tangent point slides back and forth along the top line of the rectangle. I am just going to eyeball it and get it a little bit higher, so that the curvature looks proper for what I want to design. I'm not finished with my arc, and I could add dimensions to this if I wished, but for this case I am going to go ahead and skip it, because I like the overall shape. I am going to hit Finish sketch. I'm going to then double-click with my mouse button to zoom out. And I can right-click and select Extrude from the marking menu. This will allow me to select one of the two profiles I've created.

By drawing the arc, we essentially split the rectangle into two profiles, the top part and the bottom part. The bottom part is actually the one we want to extrude, but, so I'll left-click to select that. And the Extrude dialog box defaults to one inch. I'm going to go ahead and set that to 2.75. And you can see the size gets a little bit larger. Now you don't need to understand all this, because we'll cover it in part modeling, but, one of the things I want to do here is change the direction or the type of extrusion I'm creating. Rather than move in one direction, I actually want to select Symmetric from the drop down menu here.

To extrude in the same distance in both directions. This also makes it so that the sketch plane I've created my sketch on, is directly in the middle of the part, so I can use that same plane to mirror features if I need to. I'm going to hit the green check box, and create the extrusion. Now, to see things a little more clearly, I'm going to use the visual styles button we added to the navigation bar. And select Shaded with edges. If you don't have this button, you can select the drop down arrow here, and turn on Visual styles by selecting it.

Or you can go to the view tab. To access the same menu, Visual Styles. With edges on, I can see things a little bit more clearly, and if we rotate to the front, you can see we've created the top curvature of the mouse. Next, what I'm going to do is select the bottom corner of the view cube, so that I can see the mouse from the bottom side. I'm going to select the bottom phase, and use the heads up display, the button on the far right, to create a new sketch. That will rotate me in so that I'm drawing essentially on the bottom of the mouse. And we're going to repeat the process we just did.

We're going to create a three point arc. And in this case, rather than use the midpoint, I'm going to move up a little bit higher. And left-click to start my arc there. And then start near the top of the rectangle on the other side to end my arc. Finally, I'll touch the top of the rectangle to make it tangent, and you can see I've defined the side shape of my mouse. At this point we can finish the sketch, by left-clicking on the Finish Sketch button in the ribbon bar. And then we can right-click in the graphics window to select Extrude.

In this case we're going to select the sliver that we want to remove by left-clicking. Now, Inventor defaults to wanting to add material, but in the heads up display we can change it from a Join, which is adding material, to a Cut which will remove material. And then finally, rather than extrude a 2.75 distance, we're going to use the button to the left of that value, to set it to Through All. We'll click the green check box, and our feature is created. You can now see that we have a feature on the left in the browser.

And an extrusion that cuts off the side. We're now finished with understanding how to create arcs and rectangles. So I'll really quickly finish this part off, so that you can see how we would end this part, but we'll talk about part modeling further on in the course. I'm going to select Mirror, and select the edge we just cut, and then I'm going to select the Mirror Plane option in the dialog box. I'll use the origin plane we drew on, the x, y plane, which is in the middle of the par,t as my mirror plane.

I'll select Okay, and you can now see from the top, that we have curvature on both sides of the mouse. To finish it up I'll, select a vertical edge and use the heads up display to create a Fillet. I can then select the other edges around the part, even through the model, to select all the edges I need to fillet. I'll simply drag this and eyeball to about the size I want. And then click the green check box to add the fillets. Finally, we'll finish the model off by selecting an edge on the top, selecting the Heads-Up Display for Fillet.

And changing the value to 0.5, to just make a slightly smaller fillet, and then select the green check box to create. We now have all of the features that define the basic body shape of our mouse, and we've learned about how to create rectangles and arcs while doing so.

Show transcript

This video is part of

Image for Inventor 2014 Essential Training
Inventor 2014 Essential Training

90 video lessons · 3302 viewers

John Helfen
Author

 
Expand all | Collapse all
  1. 1m 24s
    1. Welcome
      47s
    2. Using the exercise files
      37s
  2. 6m 20s
    1. Exploring major workflow steps
      2m 19s
    2. Reviewing different file types
      4m 1s
  3. 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
    5. Using the Quick Access Toolbar
      42s
    6. Using the Marking menu
      4m 33s
  4. 22m 6s
    1. Basic menu customization
      6m 40s
    2. Custom ribbon bar panels
      6m 22s
    3. Keyboard
      5m 9s
    4. Marking menu customization
      3m 55s
  5. 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. 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. 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. 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. 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. 16m 50s
    1. Projecting geometry
      7m 7s
    2. Importing AutoCAD data
      9m 43s
  11. 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. 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. 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. 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. 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. 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. 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. 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. 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. 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. 30s
    1. Next steps
      30s

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