From the course: Autodesk Inventor 2021 Essential Training

Draw lines - Inventor Tutorial

From the course: Autodesk Inventor 2021 Essential Training

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Draw lines

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- [Instructor] I wanted to take a moment and congratulate you. You're to the point in the course where we can actually begin creating geometry. And to do that, we're going to start by drawing the lines in a sketch. Lines are the most basic, simple piece of geometry that you can create. They're also the most common thing you'll use in Inventor. To create a line, we need to do two things, we need to first start a new sketch, which can be done by going to the 3D Model tab under the Sketch panel, and selecting Start 2D Sketch, or we can right-click in the graphics window, and select New Sketch. This will present the origin geometry, and we can select the XY plane to begin sketching on. You can see now we're on the Sketch tab, and we have Finish Sketch active, let's go ahead and pan down and to the left to give us a little more room to draw. Now we can start creating our lines. To do that, we can either go to the Sketch tab, under the Create panel, and select Line, or we can right-click and select Create Line from the marking menu. Let's go ahead and do that, and now let's take a look at the Heads-Up Display. You'll notice that near the cursor is the coordinates X and Y, and if you remember from the Origin movie, this sketch has an origin that is the center of the universe for this part. It's projected from the origin automatically when the sketch is created. And as we move our cursor closer to the center point, you'll notice that the values for X and Y get closer to zero. If you get close enough, a green dot will appear, and the X and Y coordinates zero out. The green dot indicates that a coincident constraint is going to be created so that we can lock the start point of our first line to the center point of the sketch. By left-clicking, we can then move our cursor to create our line. Now, before left-clicking to create the end point, let's take a look at the Heads-Up Display. As we move our cursor, you'll see that the length dimension changes, and the angle dimension changes. Right now, the length dimension is highlighted in blue, meaning we could enter a value there. We could also hit TAB, and switch to the angle dimension. I'm going to hit TAB one more time, and we can return to the length dimension, and enter one as a value. Once you have the value you want, you can hit tab, and you'll see that that dimension is entered, and a lock is added next to it. If we drag our cursor, you can see that now this line does not change the length no matter where we move our cursor. But only the angle changes. Now, we're not going to enter the angle dimension, but instead I want to show a little bit about constraints. If we drag our mouse down towards horizontal, you'll see that the line actually snaps, or kind of locks to the horizontal position. And Heads-Up Display is being shown to show that a horizontal constraint will be added. This is what I mentioned earlier when I talked about Inventor trying to automatically apply dimensions for you. In this case, I do want this line horizontal, so by left-clicking, I can create that line and continue creating new ones. But what happened, was a horizontal constraint was added and the dimension one inch was added as well. Now we can continue creating new lines. This time, I'm going to move my length out to about a half inch, it doesn't have to be exact. I'm not going to enter a dimension. This time, as we hover near vertical, what will happen is you'll see a perpendicular constraint up here. Now, I mentioned the line was vertical, but we're seeing a perpendicular constraint. And the reason for that is, Inventor will use the previously drawn piece of geometry to try to infer constraints. In this case, the perpendicular constraint is fine, when we hit 90 degrees from the previous line it applies that constraint, and we can go ahead and left-click. You'll see that constraint applied here at the bottom, and we're continuing creating lines. Now this is where things get a little interesting. If we drag this line out a little bit, and we hover towards horizontal, something happens again. This time, just like I said before, Inventor is using the previous piece of geometry to infer constraints from. Right now, we're 90 degrees from the previous line we drew. Therefore, Inventor wants to apply a perpendicular constraint. But that's not exactly what I want. In this case, I want this line to be horizontal and parallel to the line down here at the bottom. By simply dragging your cursor down and touching or scrubbing this line, when you return to a horizontal position, this time Inventor is inferring a constraint from the last thing you touched. We can always return and touch this vertical line again to get a perpendicular constraint. So at any point while you're in this command, you can touch the geometry that you want to reference. And then return, and here you can see parallel constraint is being created. Instead of left-clicking though, there's one other item I wanted to call out. And that is if we start to drag, you'll notice Heads-Up Display popping up that shows that we're directly above the mid point of this line. That comes in handy when you're drawing and you just want to quickly arrange things in a proper orientation. The dotted line does not indicate any constraint is going to be added, it's just a visual indicator that helps you when you're drawing lines. If we left-click here, I know now that this line is perfectly aligned with the mid point of the line down at the bottom. I'm going to go ahead and continue by left-clicking a line vertical to the one we just created, dragging to the far left, and again we can hover over that center point and touch it, and you don't see it because it runs right on the origin axis, but you'll notice that it kind of snaps when we get to that point. That indicates we are directly above that line, or that point. And we can left-click, and then finish off our closed profile by left-clicking on the center point again. Now that we have our lines drawn, we can right-click, and select OK to get out of the command, but we're still in the sketch. So we can use the sketch geometry to left-click and drag, and make any adjustments we might need if we made any mistakes while we were drawing. At this point, you could go ahead and add additional constraints or dimensions before you move on.

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