Start learning with our library of video tutorials taught by experts. Get started
Viewed by members. in countries. members currently watching.
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.
In this movie we are going to be focusing on the Revolve feature. To refresh, I have the Carburetor Housing open so that we can see the features we're going to be creating. In this movie we're going to focus on the Revolve and the Extrusion that are extending from the right side of the part. This time rather than starting by sketching on a face in the part we're going to return to the origin geometry, which we spoke about in an earlier movie. When we created the base extrusion, Extrusion1, we took special care in how we created that extrusion, we used the center-point rectangle, and we extruded in a symmetric way in both directions evenly.
Because of that our Origin Planes are located directly in the center of this part, and now we are able to use them to create the Revolve feature. If you open the Origin folder in the browser and hover over the planes you can see them highlighting in the Graphics window. We're going to start by sketching on the XZ Plane. Once we've selected in the browser the heads-up display allows us to create a sketch on that plane. I'm going to use my view Cube to rotate the model into a view that I prefer, and we're ready to begin sketching. One of the things you'll notice is we're sketching in the center of this part. In order to get better visibility of this sketch we're going to right-click in the Graphics window and select Slice Graphics. You could also hit F7 on your keyboard.
That temporarily removes the top-half of the part so that we can clearly see what we are sketching on. To begin creating the geometry for the Revolve we're going to project one of the edges from the existing part. In the Sketch tab you can select the Project Geometry button, and we'll select the edge on the right side of the part. You'll notice the yellow line is created because that geometry is now projected into the sketch and available for use. Because it's projected geometry it is linked to the edge that it was projected from. If this part were to change this line would change with it.
To start creating our geometry we'll use the marking menu to select the Line command, we'll lock the initial point of the line to the midpoint of the line we just projected, and we'll draw our basic shape. We'll complete the shape by connecting back to the projected edge that we just created. Now that the shape is complete we can begin dimensioning. I'm going to zoom in a bit so that we can clearly see what we're working on. I'm going to right-click to bring up the marking menu and enter the Dimension command. I'm going to select the first line we created and give it a value of 0.322.
Hitting Enter creates the dimension and updates the geometry. You notice the geometry did change a little bit, but that's okay because the important components remain. What's important here is that the lines stayed connected to the projected edge so that we can create a close profile for our Revolve. Now we're still in the Dimension command we'll select the endpoint of the shape and the horizontal line that we originally created, and give it a value of 0.252. That locates where the end of the shape touches the projected edge, and we can finish by providing a height to the end line. In this case, we're going to enter 0.163.
We now have all the geometry we need, it's been fully constrained and fully dimensioned, and we're able to finish the sketch and start the Revolve command. From the marking menu you can right-click and select Revolve, and because there was only a single profile, the system automatically selected that for you. You'll notice in the heads-up display it's moved to Axis. The system is now looking for you to select an axis to revolve around. We're going to select the original line we created as the center-point for this Revolve. The default settings for the Revolve are very similar to Extrude.
If we wanted to we could add material through Join, we could cut material away with the Cut option, or we could create an intersection between two solids with the Intersect option. Because the default is Join, and that's what we want to do, we'll leave it there. Similar to the Extrude command we do have different termination options. We could choose to select a specific angle, we could also grab the arrow on the heads-up display and adjust that angle. Simply by dragging on the screen you can see the angle adjusting in the background. For this specific revolve we actually do want the full revolve, so we'll go ahead and select the Full option to completely revolve 360 degrees.
Because the preview looks the way we want it to we can simply click the check mark to accept the settings and create our Revolve. As I mentioned earlier in this movie we were going to create two features, the first is Revolve and the second is an Extrude. Similar to the way we started the Revolve, in this case, we're going to use the origin planes again. By hovering over the planes in the browser we can see in the Graphics window what they look like and select the proper one. In this case, we're going to select the XY Plane, and we're going to use the heads-up display to create a new sketch.
Similar to the one when you were creating the revolve part of the geometry is in the way. We're going to use F7 on our keyboard to slice the graphics away to begin this sketch. We're also going to project an edge that we're going to use as a starting point. From the Sketch tab we're going to select Project Geometry, and we're going to select the end of the revolve we just created. The extrusion we're about to create needs to be centered, and we're going to use a line to lock it to the midpoint of the projected geometry we just created. In this case, we know that the center of the circle needs to be 0.168 inches away from the projected edge, enter that into the heads-up display and hit Enter on our keyboard.
We can then hit Escape on our keyboard to get out of the command, and we can use that geometry that we just created to center our extrusion. We're going to right-click and from the marking menu select the Circle command. Lock the center of the circle to the endpoint we just created and enter a diameter of 0.175 for the size of our circle. Hitting Enter on the keyboard will accept that, and you'll notice that all the geometry is fully constrained. We can now finish the sketch because we're ready to extrude. Now when we finish that command the Slice Graphics went away because it allows us to select geometry through the part, we can still launch the Extrude command and hover over where the circle is inside the part to select that profile.
By default, the value entered is one inch, which is a little too long for our design. In this case, our extrusion actually needs to be 0.375 inches long, and I'll enter that into the heads-up display, and we're ready to extrude this. Simply checking the check box will create the feature, and let's go ahead and use the Visual Styles to enable the edges. So you can see a little more clearly what our part looks like. We've now completed the Part Extrusions and the Part Revolves, and we're ready to move on to other features within this model.
There are currently no FAQs about Up and Running with Autodesk Inventor.
Access exercise files from a button right under the course name.
Search within course videos and transcripts, and jump right to the results.
Remove icons showing you already watched videos if you want to start over.
Make the video wide, narrow, full-screen, or pop the player out of the page into its own window.
Click on text in the transcript to jump to that spot in the video. As the video plays, the relevant spot in the transcript will be highlighted.