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Already up and running? This course is the next step in building your Autodesk Inventor skillset. Author John Helfen takes you through the interface and key processes of this parametric design system, including sketching, part modeling, assemblies, and drawings. Each process works in conjunction with the rest, allowing you to create parts and assemblies and document them in a way that they can be manufactured. Learn how to set up your project file; create and modify geometry; create extrusions, sweeps, and lofts; build parts with placed features and patterns of features; and create iParts and iFeatures. John also covers assembly visualization techniques, drawing views, and balloons and parts lists.
The course was created and produced by John Helfen. We're honored to host this training in our library.
As we continue to learn to how to edit sketch geometry, in this movie we're going to focus on the Scale, Stretch and Offset commands. We're going to begin by creating a new part file. We'll select New on the toolbar. Select Standard.ipt as our template and click Create. To begin, we're going to create a new sketch by clicking Create 2D Sketch, and selecting one of the origin geometry planes. Now that we're in the sketch environment, we can begin with a very basic shape. I'm going to right-click and select Rectangle.
I'll hover over the center point of the sketch and left-click. And then I'll move my cursor and define a second location for the other corner of the rectangle. Now that we have this geometry created we can look at scaling, stretching, and offsetting geometry. I ha, I don't use scale or stretch a whole lot, but it can come in handy from time to time. So, just like move, copy, and rotate which we learned about in a previous movie, these functions work in a very similar fashion. I'll start with scale.
In the Modify panel, if you select Scale, you're entered into the dialog box and you're automatically placed in the select mode. This allows you to window geometry or select a group of geometry that you wish to scale. The next item is to select a base point from which to scale. I'm going to go ahead and select the center point, or the center of the sketch, the origin point. And just like in the previous commands we learned about, Inventor is going to warn us if there's constraints added to the geometry that might be preventing it from scaling.
I'm going to go ahead and hit Yes, which will remove the constraints that are causing an issue. And as I move my cursor now, you'll see that my geometry is being scaled uniformly. When I left-click, the geometry is placed and it's in and it is all been scaled proportionally. One of the other things you might notice here, and partially the reason I don't use it that often, is one of the constraints that it removed was this coincident constraint that was locking the geometry to the origin point. If I left-click and drag on this line, you'll see that this line is no longer connected to this point.
Now because this is a rectangle, this is really easy to fix. I can either left-click and drag on that point and hover over the, the center point to snap it back into position and reconstrain it to the origin. Or, I can use the Constrain toolbar, and select Coincident. And select the point at the bottom corner of the rectangle, and the center point to lock those two into position. Now when I do that though it changes the scale of that geometry. So generally, where I use scale is when I'm importing geometry from AutoCAD and perhaps I import it and by mistake.
I import a millimeter into a inch drawing or vice versa. I might use scale to scale a bunch of geometry at once, to have it be the proper size, but I normally try to avoid it when it involves constraints and stuff I drew in Inventor. Because the constraints that are added automatically add intelligence that I typically want to keep in my sketch. But it is very simple to scale geometry using the Scale command. Next we'll look at the Stretch command. And similar to the previous command, it's going to function the same way, and it's going to do the exact same thing when it comes to removing constraints or adding constraints.
I'm going to click on the Stretch command from the Modify panel. I'm in the Select mode, and in this case I'm going to go ahead and just window the geometry here so that I can move this point and stretch it into a different location. Now you, if you remember, when I was drawing this rectangle, certain constraints were added. A horizontal constraint on the bottom, and a perpendicular constraint on this item. If I select my base point, and then pick the bottom right hand corner, I'm going to get the warning that constraints are going to be relaxed.
And when I hit Yes, I now have the ability to reposition this. What it has done, is it's broken the, the perpendicular and horizontal constraints so that these pieces of geometry can be moved. But what you'll also notice, is that the lines are no longer purple. Because of the fact that the horizontal constraint was removed. It has changed the type of geometry. So you may have to add new dimensions, in this case perhaps angle dimensions to control the exact shape of this geometry. I'm going to go ahead and undo by right-clicking and selecting Undo.
I'm going to do that a couple of times until we get back to our rectangle. Now that we're back to our rectangle and you can see that we have our purple lines again, which means we're back to where the constraints still exist, I'm going to look at the offset command. The offset command is something I use quite frequently. For example, if we go to the Modify panel and select Offset, there's a couple of settings that you need to know about that will help you get the most out of this command. First, if we right-click, there's a couple of selection options here that you may toggle on and off depending on what you want to offset.
By default, it's set to select an entire loop and to constrain the offset. And I'll show you what that means. If I go and click to get out of that command, and I hover over my geometry, you can see the effect of the loop select. By hovering over the one line it's chaining all the lines around this rectangle to select the entire loop. If I right-click in the command and uncheck Loop Select, now I'm only getting a single piece of geometry. And there's going to be times where that'll be helpful, so it's important to know about that option.
The other thing to mention is, once you've made this change, it will remain in that state until you turn it back. So it is important to not only know that those options are there, but to know that they remain in the last state. So that you don't forget it and cause confusion later on. So, I, as we go along I'll show you the outcome of, of changing that. I'm going to go ahead and select you, loop select again. And I'm going to go ahead and select that geometry, and I have the ability as I'm moving my cursor to either offset inside or outside of that line, depending on my need.
And in this case I'm going to go inside and I'm going to left-click to locate this geometry. Now I'm going to also right-click and select General Dimension, and add a dimension here. I just want the overall size of the geometry to stay locked at its current size. And the reason for that is, I want to show the constrained loop. Or the constrain option that was mentioned just a moment ago. If I left-click and drag on this corner, you'll notice that the entire loop moves in a uniform fashion.
That is the result of having the constrain option toggled. In the offset command. If, for example, I go back to the Offset command and right-click and select Constrain Offset, what you'll find is when I do my loop now it looks exactly the same up until the point where you want to change the geometry. If I right-click and select OK to get out of the command, and then grab the corner again and drag this one, you'll notice that it's not constraining the geometry beyond its initial offset.
So depending on your needs that might be perfectly okay. It's just a matter of knowing about the command and understanding what the outcome of using it will be so that you can make the proper decisions while you're designing.
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