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We're now ready to explore the sweep feature in Inventor. We're going to look at a couple of different ways to create a sweep. The first one is going to be from scratch. We're going to create the path, and we're going to create the profile, which we're going to sweep along that path. The other option, which we'll look at in the next video, we'll be using model edges as the path, rather than creating our own. To begin, I'm going to click New on the tool bar, select Standard.ipt as my template, and click Create. As I mentioned, there's two core components that are important to creating a suite feature.
The first is the path. We will begin with that. We will click Create 2D sketch and select the plane to sketch on. And while we are in the sketch environment, we are ready to go ahead and right-click and start our app. No we can use arts, we can use lines, we can use splines, but I am just simply going to use the line tool because I can free arts from within the line command. That will allow me creat essentially a path that we can use to create something like a wire. I'm going to go ahead and draw a line vertically.
I can continue drawing the line, but if you hover back to end point to the end point of the line, you'll see the dot turn gray. And, if you left-click and drag. You have the ability to create an arc. I'm going to release my mouse button to place the end point of the arc, and I'm going to find the tangent point from that circle so that I can create an additional line. I'm going to left-click to locate the end of that line, and I'll repeat the arc command by going back to the end point. Left-clicking and dragging to create my next arc.
And then finally I'll drag straight down to create a vertical line off the end. I'll right click and select OK to get out of the command. And if you zoom in a little bit you'll notice that I didnt quite get that final tangent constraint here. Between this line and this arc. To add that constraint, I can go to the Constraint panel in the Sketch tab and select Tangent. Select the arc, and then select line to add that constraint and make those two components tangent. Next, I can zoom out to make sure my line is correct.
And, if I want to, I can create dimensions here by right-clicking and selecting Create General Dimension. I can select the center point of the circle and the end point of the line and I can set that to 0.5. Hitting Enter locates the model and the sketch is updated. I'm going to go ahead and stop there. You don't need all the dimensions for this example so it's up to you if you want to practice by adding some dimensions. You're more than welcome to. But we have enough information. Right now what we've done is created an open-ended line, which we can use as a path.
If I hit Finish Sketch, I'm returning to an isometric view and I can look to create my profile that I want to sweep along that path. What's important about the combination of that path and profile, is you want your profile to intersect your path at, at least one point. I'm going to go back to my origin geometry and find the plane that is on the bottom here. The x z plane. Which if we select that and look at it from the front view, it perfectly intersects the end point of this line. And I'm going to go ahead and create a new sketch on that.
What that does is it allows me to use the center point of this sketch which does intersect the end point of the line in order to create my profile that I'm going to sweep. I'm going to right-click in the Graphics window and select Center Point Circle. I'm going to hover over the end point of the line or the center of the sketch and left click to locate the center. And I'm going to enter a value 0.125 for my circle. By right-clicking and selecting OK, I can get out of the command. And I can finish the sketch and go to my Home view to see the results.
I now have everything I need to actually create the sweep. I have a sketch one. That includes an open ended path and I have sketch two which is the profile I want to sweep along that path. And they do intersect each other, the circle sits directly on the end point of this path line. If I go to the Create panel in the 3D Model tab and select sweep. You'll notice something happens. Just like in the extrude, revolve and loft features. Inventor gives me the option to pick the profile I want to take action on, and the path I want to use with that profile.
Since we only have one profile this one closed loop circle. Inventor automatically selected the profile for me. Had there been multiple circles here, it would have allowed me to pick the ones I wanted to sweep. I'm now ready to select the path. And, if I left-click on the path we've created, you can see a preview of what the result will be. Just like te extrude and revolve features, we do have settings that are pretty standard across all of our features. for example, we have the ability to select the type of output, whether it's a solid or a surface.
We have the ability to select whether we're going to join, cut or intersect material, but in this case since it's the very first feature or base feature, it defaults to new solid. That's going to happen for the feature of any part. Additional suite features will allow you to join, cut, or intersect material, and we'll look at that in the next video. We also have the option similar to a loft command, to use a path or use a path with a rail or a guide surface. We are not going to look at those that are a little more advance for a essentials course but just know that they are available if you want to do your own research.
We also have the ability to follow the path exactly or sweep in a parallel fashion. We are going to stick with the path option right now because it is the most basic and it is what you are going to use most of the time. By clicking OK, you can see that we've created our sweep feature in the browser. And because it's a sketched feature, it has consumed the two sketches that were required to create it. Next, we'll look at how to use model edges as your sweep path.
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