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.
In a previous movie when learning about rectangles and arcs, we created the basic shape of a mouse. Well, it's not the most fancy mouse, we can spice that up a little bit or change the design by using splines instead of arcs. Here, I have a sample of the next item we're going to create. If you look at it from the front, you can see rather than just the arc shape, we actually have a flowing organic line. That's the spline. If we look at it from the top, we have the same thing on the sides as well. I've created a basic Exercise file that starts out with a primitive shape, that's set up so that we can continue the process.
To begin, we're going to select the side of the shape, and use the heads up display to create a new sketch. That places us in the sketch environment, you can see we have the Sketch tab. And on the Draw panel, we have the ability to create splines. If you select the drop down, you can see that there's three different options. There's a spline with control vertex, spline interpolation and a bridge curve. We're going to work on creating a spline with a control vertex option. We can begin our spline by left-clicking anywhere on the vertical line on the left.
I'm going to use the midpoint, indicated by the green dot, which also means inventor is going to add a coincidence constraint, locking the beginning of the spline to that location. Now, a control vertex spline is essentially a series of points that control the flow of the line through the sketch. If I move my cursor up above the shape overall and left-click, I'll create the first control point. You can see there now that the point controls the spline, and I can left-click to continue creating control points along the sketch.
I'll finish by left-clicking on the vertical line on the right, and then selecting the green check box to create the spline. Once the spline is created, you have full control to add new points, move the existing points, delete points, and make modifications to the spline overall. Generally, I use these points to control the overall shape. If you want to get very specific about it, you do have the ability to dimension the angles of these control lines and dimensionally control points themselves.
I'm not going to do that at this point, because what I'm most interested in right now is the overall shape. That shape generally looks close to what i'm looking for, and I can always return and make edits to it later. But, i'm going to finish my sketch here. I can now right-click in the Graphics window and select the extrude option from the marking menu. And I have the ability to select either of the profiles that were created by drawing the spline. I'm going to select the top half because that's what I want to remove, and what you'll find is Inventor wants to add material.
I can use the Head's Up display in the extreme command to change from a joint a cut. And you can see if here my default one inch value doesn't cut all the way through the part. I'm going to use the drop-down menu to the left to select Through All as my termination type. I can select the green checkbox and the features created. If we look at it from the front view on the View Cube, you can see the overall shape has been defined by that spline. I'm going to hit my Home button. We're now going to select the bottom corner of the view cube to view the model from the bottom.
We're going to select the bottom flat face and use the heads up display to create a new sketch. By doing this we're in a position now where we can divine the shape on the side of the mouse. And we'll do that again with this spline. From the Draw panel on the Sketch tab, I'll select the Spline tool. I'll start my point by selecting a position on the vertical line on the left, and then I'll create control points. And you can create as many as you feel you need. The fewer you use, the more control you're going to have overall with the line I think, at least controlling the smoothness.
But you can always add as many as you need, and you can add and remove them after the fact if you need to as well. If I were to right click on the line, I do have an option to insert vertex, which would allow me to add additional points if needed. I'm going to lay out the basic overall shape, and I know I want this to be not entirely straight but not super curvy either. So I'm going to go ahead and manipulate this a little bit to get a line that defines what I think is a good side view of the model. I'm going to finish that sketch by selecting Finish Sketch on the ribbon bar.
And I can right click in the Graphics window to select Extrude. I'll select the sliver that I want to remove, and change the head up display to cut material rather than join material. I'll finish up by setting the termination to be through all, which cuts all the way through the model. And I can hit the green check box to accept that, and I now have another extrusion in my browser. Now that we've seen how to create splines, I'll really quickly use the mirror command to mirror the extrusion we just created. I'll select mirror plane in the dialog box, and select the original xy plane in the center of the model.
I can hit OK to mirror that, and then we can finish up the model by selecting edges to create fillings. I'll continue selecting multiple edges, you can even select through the part. And then I'm going to enter 0.625 as my value for my fillet. I'm going to click the green check box to accept that. And finally, I'll finish off by selecting the top edge, selecting Fillet from the Heads-Up Display, and setting the value to 0.5. Which gives us a nice organic shape overall. To see more clearly, we can turn on shaded edges by going to the Visual Styles drop-down in the navigation bar and selecting Shaded With Edges.
If you don't have this button, you can use the triangle at the bottom of the menu bar to select visual styles and enable it. It's also available on the view tab here in the Appearance panel.
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.