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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 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.
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