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This course introduces you to the interface and key processes of Inventor, the parametric design system from Autodesk. Author John Helfen covers sketching, part modeling, assemblies, and drawings. These tasks work in conjunction, allowing you to create parts and assemblies and document them in a way so that the manufacturing process proceeds faster and more efficiently.
The first part modeling feature we're going to focus on is extrusions. On the screen, you'll see the part that we're going to build throughout this chapter. I'm going to roll the End of Part icon back to just below Extrusion 8. On screen, you'll see what we should end up with at the end of our extrusions. We're going to go ahead and create each of the eight extrusions that make up this part. When I begin part modeling, I like to look for the biggest or most pronounced feature, or the item that has the most things attached to it as my base feature. That way, I have something solid I can build out from. In this case, I see it as being this cube, and that's where we're going to start.
I'm going to start a blank file to begin this process. From the Application menu, you can select New > Part to create a blank part file to start from. I'm going to create a new sketch by right-clicking and selecting New Sketch from the Marking menu. Because this is the base feature, the origin planes are displayed, and I'm able to select a plane to sketch on. Now, because this part is overall fairly symmetric, I'm going to draw my initial rectangle in a specific type of way so that we can leverage the origin planes as we model things throughout this chapter.
I'm going to start with the Rectangle command, but I'm going to select a specific type of rectangle. I'm going to use a Two Point Center Rectangle. By doing this, the first point I select is considered the very center of the rectangle, and as I drag out, my heads-up display allows me to add dimensions to this. In this case, this cube is going to be 0.692 in width. I'm going to hit tab on my keyboard to move to the next dimension, and enter 0.757. I'm going to hit tab on my keyboard again, and then Enter to actually create the rectangle.
You'll notice by using the heads-up display and the center point origin that was projected to the sketch, I was able to fully constrain and lock this rectangle down just using the heads-up display. I'm now ready to create my first extrusion. I'll right-click and select Finish Sketch, and I return to the modeling environment where I can then right-click and select Extrude. Now, I know this extrusion has a height of 0.518, and we're going to extrude it to a distance. But before we do that, I wanted to talk a little bit about the heads-up display, and the other things you see on the screen.
You'll notice the heads-up display here near my cursor, but also on the screen, you'll notice the Extrude dialog box which is hidden. Clicking on the dropdown arrow exposes the dialog box that actually controls this. It's up to you whether or not you use it. I prefer to use the heads-up display. But while you're learning, it might be worthwhile to actually use the Extrude dialog box. When extruding, there's a few different options that you need to input to determine the geometry that's created. You have to pick a profile, which we did right when we started. If there's only one profile in a sketch, the system automatically selects that profile for you.
The next option is Output. In this case, we're actually creating a solid model, the other option is Surface, but we won't be covering that in this course. Because it's the base feature, we have limited options here. These buttons that are grayed out in the center are options for Join, Cut, and Intersect. But we'll cover this in later extrusions. By default, the very first base feature is creating a new solid, and that's checked by default. Under the Extends area, we have the ability to select different types of termination. We can say extrude to a distance, extrude to a specific item, or between two items.
We have the ability to enter a distance, and then also a direction. Now that we've seen this, I'm going to go ahead and collapse this and return to the heads-up display because all the same information is available in the heads-up display. You have from the dropdown menu a Distance, the option to select to a specific point or face, or between two faces. We have the ability to select our profiles which again was already done for us. We have the ability to select whether we're going to do solid or surface. In this case, we have Join, Cut, and Intersect, but because it's our base feature, we're going to create a new solid. We have our directions.
And in this case, because its symmetric part, and we used the center rectangle, I'm going to actually use Symmetric. This will allow me to perfectly center this part so that we can appropriately use the origin planes in future extrusions. And last but not least, we have the option to cancel this command or accept the inputs. In this case, before I actually accept this input, I'm going to set the corrected dimension, in this case, 0.518. I'm going to hit Enter on my keyboard to accept that part, and now we have our first base feature which you can see in the browser.
When we hover over it, it highlights in the graphics window. Now, before we continue, I'm going to do a couple of other things. I'm going to turn on my Visual Style to show shaded edges. I'm also going to reorient this model a little bit from the view Cube standpoint so that it's in the proper orientation for continuing. I like to have my XY plane as the flat surface and Z pointing straight up. Once I have the orientation set, I can right-click on my Home button, I can set Set Current view as Home, I'm going to fit it to the view, and I'm going to select the Right view, and change that to represent the Front view.
I can do that by right-clicking on the view cube, selecting Set Current view As and then Front. When I click my Home view, I now have the model in the proper orientation to continue. This is really a personal preference, but I think it's worthwhile for everybody to get used to how to reorient the model to fit their design preference.
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