Viewers: in countries Watching now:
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.
Now that we've learned how to create extrusion, we're ready to move into revolves. The nice thing is, because you've already learned how to create extrusions, a lot of the interface components are going to be exactly the same. Let me create a new part by clicking New on the toolbar, selecting standard.ipt as my template and clicking Create. Now that we're in a blank part file, we can begin by creating a new 2D sketch. We'll click Create 2D Sketch. And select the face to sketch on to enter the sketch environment.
We're now ready to begin creating our shape that we want to revolve. And we're going to do this a couple of times so you can see a few different options. But just like the extrude feature, the base feature or the first feature created in a part is going to have slightly different settings. Than future extrusions or future revolves within each part. I'm going to go ahead and create a rectangle. Starting at the center point of the sketch. And we'll set the overall width to be 0.5. And hit Tab on the keyboard. And we'll hit 1 as our value for the height.
And then we'll hit Enter to create that rectangle. And we also create the dimensions on the fly. Now that we have the shape completed, we can finish the sketch, and enter the Revolve command. We can right click in the graphics window and select Revolve from the Marquee menu. Or you can go to the Create panel and select Revolve there as well. I'll select Revolve from the Marquee menu. And just like the extrusion, because there's only one sketch here, or one profile, Inventor has automatically selected that for me.
It has then put me into the Access Selection mode, which allows me to pick what I want to revolve around. For example, if I select the vertical edge, I'll get a cylinder standing on end. If while still in the Access command, I hold Shift+down on the keyboard I can un-select that axis as well and for example, select a different one. So depending on the axis you select, you're going to get two very very different shapes. They'll both be cylinders, in this case, because we're revolving a rectangle.
But they'll be revolved in different directions. Again, if you hold Shift+down, if you're in the axis mode and you hold Shift+down, you can de-select that, and select a new one. Just like the extrusion, I also have the option to create different items. I can select an output of Solid or Surface. I can do Join, Cut, Intersect, or New Solid. Since this is the very first feature, I'm limited to only doing a New Solid. But additional Revolves would enable all of these. And, finally, I would have a direction here.
But since this is a Full Revolve, I don't have those options currently. If for example, I change the angle from Full to 90 degrees or 60 degrees, you can see the model update. And I do have a direction now. I can flip the direction the revolve is going to to take place in. I can make it symmetric, essentially on equal on both sides, or asymmetric, just like we could with the extrusion. I'm going to go ahead and select the default direction. I'll select the termination type.
And you'll, can see I have Angle, Full, and a few other options. Like Between two faces or planes, or between a Fit, or To a selected face or plane. I'm going to go ahead and select Full. Angle and Full are most likely what most people are going to use. And I can select the green check mark to indicate I'm ready to create that feature. Since I created this model directly in the center of the origin, I can use one of the origin planes to create our next revolve. When we rotate into the sketch mode, we can adjust our view so that it's the way we want to view it at.
We can hit F7 on the keyboard which will slice the graphics. So that we can clearly see what we're going to be sketching on. And finally, because this runs through the center of the part, I'm going to use the Project Cut Edges option. To project all of the edges that have been sliced by the workplane running through the center of the part. What this does is allows me to create a new profile that I can revolve. In this case, we're going to go ahead and create a small groove that's cut around this cylinder.
Perhaps for an o-ring to sit in or many other reasons. But I'm going to then right click and select General Dimension from the Marking menu and I can start to define the overall size of this item. I'm going to say that this is 0.125 thick. We're going to say that it is 0.125 deep. And we'll set it to 0.125 off of the top edge. You can now see that I have everything fully dimensioned. But the one thing that I don't have is an axis to revolve around.
I could draw a line in. I'm going to go ahead and do that. From the center of this bottom point to the top of the model. And I'm going to select OK. And when I finish this, you'll see that I get my graphics back and I'm rotated back into a 3D model. I can right click in the graphics windows and select Revolve. Like the extrude, because there is multiple profiles that I could take action on, Inventor's placed me in the profile mode. Where I can select the item I want to specifically take action on.
I'm going to select the rectangle. And then, I can go into the axis selection mode. This allows me to either select the sketch line that we created as an axis. Or, because I know this geometry was created in the center of the origin geometry, I can use the y-axis as well. When I do that I can then continue on selecting different options. For example, just like in the extrude, I could enter a specific distance. But before I do that, I'm going to select the type of revolve I want to do.
In this case rather than Join material, I want to Cut material away. This will allow me to see a preview of what we're going to receive. And we can talk a little bit more about the termination type and the distance. By default, these are the same things that you're going to see in an extrusion or very similar anyway. An angle is just like the distance extrusion and the full is like through all, roughly. If I select an angle, it defaults to 90 degrees and I can enter a specific value. I could say I want this to go 180 degrees and you'll see that it revolves all the way around the back side.
If I select 270 degrees, you can see that it's working its way around the circle. By selecting full, it will complete the full 360 degree cut. By selecting the green check mark. I'm ready to enter all these values and create the feature. You can now see in my browser I have two sketched features, both of them are revolves. And at any point I can go back and double-click on any of the sketches. In this case I'll hit F7, just so I can see a little more clearly. And I can update any of these dimensions.
Perhaps we want to make this groove a little bit deeper. I can enter 0.25 And when I finish this sketch, you can see that the model is updated and the groove is a little bit deeper.
There are currently no FAQs about Inventor 2014 Essential Training.
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.