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Move, copy, and rotate sketch geometry

From: Inventor 2014 Essential Training

Video: Move, copy, and rotate sketch geometry

Now that you've learned how to create geometry, we can circle I'm going to start a new part file by clicking This will create a new part file for us. Now that we're in a blank part file we need to start a new sketch. I'm going to start by creating a 2D rectangle, and I'm going to create But, once I have geometry you'll notice everything is green If you go to the Modify panel, and select Move, you can see that With this rectangle disconnected from the center plane, When I select geometry by left clicking and dragging and I'm going to go ahead and undo that and show how to use the Copy command.

Move, copy, and rotate sketch geometry

Now that you've learned how to create geometry, we can circle back and talk a little bit about how to edit that geometry. I'm going to start a new part file by clicking New on the toolbar, selecting Standard.ipt, and then hitting Create. This will create a new part file for us. Now that we're in a blank part file we need to start a new sketch. We can do this by clicking Create 2D Sketch on the toolbar, and then selecting one of the planes from the origin geometry that is presented. We're now in the sketch environment, and we can talk a little bit about how to edit geometry.

Specifically we're going to look at Move, Copy, and Rotate. Now before we get started, I'll let you know that while I'm sketching in Inventor, I don't use these tools all that often. And the reason for that is, Inventor has intelligent features like constraints and dimensions that can actually move geometry or position geometry. And most of the time, it's more efficient that way. The intelligence really is beneficial in Inventor. But, there are times that you may want to use Move, Copy, and Rotate where it is appropriate. Generally, when I see people using it, it's after they've imported 2D geometry from AutoCAD.

And they want to move a large piece of geometry, perhaps out of the way so that it can create a profile and extrude that, and delete a bunch of other information. It's more about cleaning up data than it is moving geometry in a simple way. I'm going to start by creating a 2D rectangle, and I'm going to create that out in space, which is not how I would normally start. I would normally recommend that people always start geometry from the center point of the sketch. It just makes editing sketch geometry more predictable. But, once I have geometry you'll notice everything is green which means it's unconstrained and it can move in any direction.

If I grab a line, I can click and drag it and it maintains its general shape. I'm just adjusting the size. Same with the side vertical lines. And if I grab a point, I have more of a free form move where I can scale the size of this. Now, while I'm doing this drag motion by holding down the left mouse button and dragging the mouse. You'll notice when I hover over the center point, Inventor gives me a heads up display indicating that it's going to add a coincident constraint. When I release the mouse, you'll see that these two lines are now purple, indicating that they're locked into position by something.

In this case, the fact that we just locked the end point to the center of the sketch. I'm going to go ahead and right-click and undo that, and show you how you can also move it using the Move command. If you go to the Modify panel, and select Move, you can see that the Move dialog box is presented, and we're in the mode to select geometry. I can simply select the entire rectangle, or if I needed to I could select only individual pieces of that geometry. Now that we have the geometry selected, we can go to the Base Point option, which allows us to select a point to move from.

Once we have that, I can move over to the center of the sketch and you'll notice it sort of snap into place. So it is locating the point exactly on the center point of the sketch, but you'll notice here, I'm not getting any heads up display indicating that a constraint is going to be added. And if I left-click, you'll notice this time, that the geometry did not change color, and if I were to grab one of these lines and drag it, it's not locked to the center point. While the Move command allowed me to move geometry in a group all at once, it doesn't apply automatic constraints, so there's good and bad to it depending on your need.

With this rectangle disconnected from the center plane, I'll talk a little bit about the Copy command. And this one I use a little more frequently. And the reason for that is, if I were to select this rectangular geometry and use Ctrl+C, and Ctrl+V on my keyboard, it pastes the geometry slightly offset from the original, which is normally fine but it makes it a little bit hard to select the geometry. When I select geometry by left clicking and dragging and moving to the left, I get what's called a crossing window. That'll select anything the box crosses.

If I do the exact same thing from the opposite side, I left-click and drag, I get a solid line window. And this only selects things that are completely engulfed or consumed surrounded by that window. But even in this case, doing it that way, I still pick up this line here, which then I would then have to hold Shift down, and deselect it. But you can see I also have points, so clearly a selection can be a little bit difficult if you use the Ctrl+C and Ctrl+V. I'm going to go ahead and undo that and show how to use the Copy command.

It works a lot like the Move command. I'm going to go to again to the Modify panel and select Copy. And when the dialog is open, I'm in the Select mode, which allows me to select the geometry I want to copy. And just like the Move command, I can select a Base Point. Now, I'm moving my mouse around, and you can see that the geometry follows the cursor. And each time I left-click, I'll get a copy of that geometry. This isn't quite as handy when you're copying a rectangle because rectangles are really simple to create. But if you had something like a keyway, or some slightly more complex sketch using the copy in this fashion might be a little bit easier if you need to create multiple pieces of that same shape.

I'm going to go ahead and again undo to backed out of those copies. And now I'm going to talk about Rotate, but before I do that, I'm going to go ahead and drag this geometry and lock it back to the center point. There's a couple of things I want to call out here. When I created this original rectangle, Inventor added automatic constraints. If I right-click in the graphics window, and select Show All Constraints, you can see that I have a parallel constraint, I have a horizontal constraint, another parallel constraint, and a perpendicular constraint. These are constraints that Inventor automatically added.

Now, by definition, a constraint is essentially a rule that restricts motion. So this horizontal constraint is going to cause us problems when we try to rotate. But I wanted to call that out because that's okay, and I don't want people to get scared by warning messages that come up because they, they can be common from time to time, and they're just normal part of design. So when I go to use the Rotate command, I work through essentially the same process I did with Move and Copy. I'm in the selection mode. I can select a bunch of geometry and then I can go select a center point, that I want to rotate around.

Now when I left-click on this center point, Inventor's going to bring up a warning message. And this isn't really a problem, it's just letting you know what I just explained. That the geometry being edited is constrained to other geometry. And it's asking if you'd like to delete that constraint or any of the constraints that are blocking this motion. And in this case I'm going to go ahead and hit Yes. Now what's happened is Inventor has essentially deleted that horizontal constraint to allow this geometry to rotate. The thing about the Rotate command and the relaxing of constraints that you want to be careful with, is that sometimes Inventor is adding automatic constraints that you don't want to delete.

Or, it might be constrained to other geometry that might be preventing motion. You just want to be a little bit careful about understanding the constraints that have been applied to that geometry, before you just delete or relax those constraints.

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This video is part of

Image for Inventor 2014 Essential Training
Inventor 2014 Essential Training

90 video lessons · 2934 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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