Join John Helfen for an in-depth discussion in this video Create a sweep feature, part of Autodesk Inventor 2018 Essential Training.
- [Voiceover] We're now ready to look at the sweep feature. In order to create a sweep, we need two things. We need a profile that's gonna be swept, and we need a path that it's gonna be swept along. To begin, we need a blank part file, which I have open on the screen. I'm gonna right click and select New Sketch, and I'm gonna select the XY plane to sketch on, and what we're gonna do here, is we're gonna create a path that we can sweep up a profile along. I'm gonna start by right clicking and selecting Create Line. Hover over the center of the sketch and left click to start the line, and I'm gonna drag upward, to about .75 inches.
It doesn't have to be exact, and I'm gonna left click. Now, I could continue creating lines just by left clicking anywhere, but I'm gonna show you a trick. I wanna actually create an arc here. If you hover your line back to the end point on the previous line, you'll notice a small gray dot appear. When you see that, if you left click and hold your mouse button down, and then drag your mouse, you'll notice you can create an arc, while in the line command. I'm gonna go ahead release my mouse button, and I'm back to creating a line again, so now I can go ahead and move my cursor up until I see tangency show up on the heads up display, and I can left click to create my second line.
We'll repeat that process one more time to create an arc. Again, return to the end of that line until you see the gray dot, left click and drag, and you'll create an arc. Now I'm gonna drag this arc down a little ways until I see this heads up display pointing towards the center of the arc When I see that, I know that I can release my mouse button, because if I continue creating a line straight down, it will be tangent and parallel to the original line we created, the very first line over on the left.
If I left click, I can create that. Then I can right click and select OK to get out of the command. I now have it on open profile, that I can use, to sweep a profile along. We'll go ahead and finish the sketch, and double click the middle mouse button to zoom in. We're now ready to create the profile that's gonna be swept, and in this case, there's one other thing that's important. You always wanna create the profile that's gonna be swept, at a point that's at the end of the path. Now I could go to the work features panel and create a work plane that is perpendicular to this line at this end point, but because we created this geometry at the center of the sketch, I know that we have a work plane already, at this point, and i's in the origin geometry.
If we return to the browser, and expand the origin folder, we can find the XZ plane, which is the plane at the end of that line, and we can left click on it, and we can use the heads up display to create a sketch on that plane. We're now in the sketch and we can go ahead and right click, and select Center Point Circle, and use the center of that sketch to create a 1/8 inch circle. We'll enter .125 as our value, and hit enter. If we finish this sketch, you can see we now have what we need to continue.
We have a profile, and we have path. To create the sweep, we need to go to the Create panel in the 3D Model tab, and launch the Sweep command. Now in the Sweep dialogue box, most of this stuff at this point is gonna look very familiar. We need to select a profile, which has already been done for us, cause we only had one. We've entered the path selection tool, and I'm gonna go ahead and select the path we wanna sweep along, and we get a preview of what we're gonna get. We have an output option for solid or surface. We'll keep the default, and then we have different types of paths.
We have the default path, which is what we're gonna use, and we also have a guide rail and a guide surface option. Those are a little beyond an essentials course, so we're gonna stick with the path option. From an orientation stand point, for this type of sweep, we're gonna go ahead and leave the path as well. We'll skip the parallel option for an essentials course. If you go ahead and click OK, you can create that geometry and you can see that in the browser, we have Sweep 1, and just like the loft, if you click the plus symbol next to it, you can see that it's consumed the sketches that were required to create it.
Sketch 1 is our path and Sketch 2 is our profile. Now what I'm gonna do is show you one other thing, cause in most cases, sweeps tend to be circular in nature. They tend to be O-rings, they tend to be wires, and that's not always what you're gonna be creating. Most of the time it is, but nobody said that this profile had to be a circle, so what we're gonna do, is we're gonna go and edit Sketch 2 by double clicking on it in the browser, and I'm gonna right click on this circle, and convert it to Construction.
What that means, is Inventor's gonna ignore that it exists when it creates a feature. Instead, what I'm gonna do, is I'm gonna return to the Create panel, and click the drop down arrow under Rectangle, and select Two Point Center. What this will let us do, is create a rectangle by defining its center point, which in this case will be the center of the sketch, and one of its corners. Now that we've created that, I'm gonna go ahead and finish this sketch, and you'll see that the geometry already updated because we turned off the circle, by making it construction, and then we created one single profile.
Inventor just swapped those profiles out in the background. We could always go back and repeat that process, and update this, but what's important here, is to know that it doesn't just have to be a circular profile. You could use rectangles or squares, or any real shape that you wanna create.
- Reviewing interface changes
- Projecting and importing geometry
- Working with Autodesk AnyCAD
- Understanding part modeling
- Building parts with placed features
- Working with partial chamfers