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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 the previous movie, we learned how to create offset work planes. Now we're going to look at some of the other options available, beyond just offset. Again, we'll return to the 3D Model tab to the Work Features panel, and we'll look at the work plane option again. And by clicking the bottom half of the button, Inventor will display the entire list of work planes that can be created. I'm not going to cover all the work planes, because once you understand how to create a few of them, they all work the same. And generally that should give you the essential skills you need to create these work planes.
As you improve your skills in Inventor, I do recommend that you come back and try creating each of these types of work features, even if you don't need them. Just so that you can understand how to create them and keep them in mind when you're designing. We're going to start by looking at parallel to a plane through a point. In the previous example with the offset work plane, since there was only one type of input needed, a plane, Inventor limited the selection capabilities to only select planes. In this case, we're going to do parallel to a plane through a point. So, we have the ability to select planes and points this time.
You can see at the intersection or end points of lines, and at the midpoint of lines, you can make selections. I'm going to go ahead and select the angled face here, and as I hover over specific points beyond that, you'll see previews of the work planes that could be created. You'll also notice that because the first input was a plane, I can no longer select planes, because you only need one plane and one point to create this type of work plane. So I'm going to go ahead and select the midpoint of this line. And if we look at it from the top, you'll see that this plane is now parallel to that face that we selected.
And it runs right through the midpoint of this line. If I return to the Home view, we can look at couple other options. I'll select the drop down menu again. And this time, we'll look at the mid plane between two parallel plans. This comes in very handy when you want to mirror things or create a center plane through a part. And and it requires two planes. More specifically, it requires two planes that are parallel so that it can create a mid plane between those two planes. I'm going to start by selecting this front edge, and you'll notice after selecting it, I can no longer select any of the three planes on the side or on the angle or on the top.
And the reason for that is, Inventor needs another parallel plane. In this case, there's only one other plane that's parallel to this one on this model. And you can see if I hover to the other side, it'll automatically selects it when I hover above it. By left-clicking and then selecting the top view, you can see that the work plane, Work Plane 2 in the browser, is actually cutting directly through the center of the part. The final one I wanted to look out would be the angle to a plane around an edge. By selecting this, Inventor changes the input types to be faces, or planes, and edges, instead of points or just planes.
I'm going to go ahead and select the angled face here. And again Inventor lets me preview my inputs by just hovering over specific lines, and I'm going to use the vertical edge at the end of this model, and by default Inventor sets it to 90 degrees. That's what you'll use most of the time, but you do have the option to change that angle. For example if I use 45 you can see that the angle updates. And it's up to you to decide what works for you for your design. I'm going to return it to 90 and select the green check mark to enter that value and accept that creation of the work plane.
And when we look at it from the top view, you can again see that it's 90 degrees from the face that we selected and it runs through the intersection of the two lines here. Which is essentially the vertical edge we selected. Now the other thing that's important to remember is the inputs you select are linked to the model. This is important because it can be either incredibly powerful or incredibly frustrating, and I want to make sure it's more powerful than frustrating for everyone. So, if we were to select this top face and edit this model, and make it a little bit longer or a little bit wider, and the distance doesn't really matter in this case just as long as you can see the change.
And the reason I wanted to show this is because if I were to toggle back and forth between undoing that change and redoing that change you can see how the work planes update accordingly because they're linked indirectly to the model. Again, if you know that this is going to happen it can be very powerful. You can build intelligence into your model but if you're not prepared for it, you could design something on a work plane, expecting that it's not going to change, but then when the model is edited it could potentially cause problems.
So as long as you know that ahead of time you should be okay. Now that we've learned how to create those with Inventor's auto-selection tools turned on, essentially by selecting one of the items from the list other than this default plane. I want to circle back and talk a little bit about that. I'm going to select Work Plane 1, hold Shift down on my keyboard and select Work Plane 3 so that they're all selected and then I'm going to hit Delete on my keyboard. And the reason I'm doing this is I want to show that you can create all those work planes with the default plane tool. And I'll let you know that the only time I ever drop this menu down to select these options is when I'm training people who are new to Inventor.
Because once you understand how to create all of these you can do them all from this single command. If I click the default plane tool we'll start with the first plane we created which was, parallel to a specific plane. In this case, I select the angled face and through a point. If I look at it from the top view, you can see that it created that same plane that we had before. It's parallel to this line and it runs through the midpoint of this line. Because the default plane doesn't limit the selection tools, you can select planes, edges, or points all in the same command.
So if I select this first face, I can select through an edge, I could select through a point, or in this case, if I hover towards the back of the model, I'll get the plane on the opposite side of the model, and I'll get a work plane through the center. If you look at it from the top, Work Plane 5 is now directly through the center of this part. And then finally, we'll enter that command one more time. We'll select the angled face and the vertical edge. We'll leave it at 90 degrees. And when you click the green checkmark, you'll see that Inventor now has all three of those exact same planes, but you only used a single command to create them.
So once you get the hang of the features, again, you'll probably end up just using this default command most of the time.
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