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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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