Join John Helfen for an in-depth discussion in this video Add control to a loft by Create rails, part of Autodesk Inventor 2018 Essential Training.
- [Voiceover] In the previous movie we learned how to create the shape you see on the screen, and we also looked at the Conditions tab in the Loft tool in order to learn how to control the flow of the 3D shape through the profiles. And that might work for a lot of cases, but when you really want to have full complete control over the shape of your 3D model through the profiles, the only way is with rails and that's what we're going to create here. What we're going to do is we're going to start by deleting this loft. If we go to the browser and right click on Loft, we can select Delete.
In the Delete Features dialog, if we were to simply hit OK, we would delete this Loft and everything related to it. However, if we uncheck this checkbox consumed sketches and features, and then click OK, all of the geometry that was used to create the feature remains, even though the feature has been deleted. Now we need a sketch that will hold our rails. We'll go ahead and right click and select New Sketch and rather than offsetting a plane, we're going to return to the origin geometry, and click the plus symbol next to the folder and hover over the planes until we find the x y plane that runs right up through the center of all the profiles.
We'll left click on that, and then we'll click the home view in the view cube to return to an isometric view. The reason for this is I want to talk a little bit about what's important when creating rails. The number one most important thing is that each rail must intersect the profile at a single point. The way to make this easy is to project those profiles to the rails sketch. If we return to the Create panel, we can select Project Geometry, and then we can simply select on each of those profiles.
You can see each of them is projected to the sketch plane as a flat, yellow reference line. I'm going to right click and select OK to get out of the Project Geometry command, and as I mentioned, the yellow lines are reference geometry. And I'm going to leave that as is, but this is going to cost us a problem when we're creating a rail and that's okay, I want you to see this because as you go off and practice on your own, you may very easily run into this and it's easy to fix so I want to show you how to do that. To create the rails we're going to use splines.
The Spline tool can be found in the Create panel, under the Line command. We'll click the drop down arrow below Line, and I'm going to select Spline Interpolation. We're going to rotate to the front view and as we hover along this line on the bottom profile, there'll be a point where a green dot pops up. This is Inventor finding the end of the reference line in that sketch. The green dot indicates that a coincident constraint is going to be created, and that's what we want. So we'll go ahead and left click, and then we're going to left click somewhere between the first and second sketch.
Next, we'll go ahead and find the endpoint on the middle sketch, left click, we'll create a point in between the second and third sketch and then we'll finish up at the end of the reference line in the third sketch. Finally we can click the green checkmark, and our spline is created. Now, the spline can be modified by simply clicking and dragging on those points. When I do that, you'll notice that there are handles that come up. They're very fine, gray, outlines and that's because they're not active by default.
If you want to, you can right click on a specific point and activate that handle, and that will allow you to click on that point and then use that handle to truly control the curvature of that line at that point. Now I'm going to go ahead and undo cause I don't want that handle right now. I'm going to undo one more time to turn it back off and now we're ready to mirror this rail. First we need to create a centerline. I'm going to right click and select Create Line. I'm going to hover over the center of the sketch and left click, and I'm just going to draw a line straight up a little ways, left click, and then right click and click OK to get out of that command.
I'm going to go ahead and select that line and then right click on it and convert it to a centerline. And now we're ready to mirror that rail. And you'll understand why we mirror it in just a moment when we create the rail. But let's go ahead and move up to the Pattern panel in the Sketch tab, and select Mirror. By default, the selection tool is enabled and we can simply select the spline. We can then go select the Mirror selection tool, and select the centerline we created. With both of those selected click Apply and you can see we now have a rail on both sides, and before we exit the command, you can also see that we have symmetry constraints on each of the points within the spline.
That's incredibly important because that way, if you make a change on one side, it'll be reflected on the other as well. I'll go ahead and click Done, and we now have our mirrored rail. If you left click and drag on any of those points you can see the symmetry in action. Let's go ahead and finish that sketch and we're now ready to create our Loft. If we return to the Create panel in the 3D model tab, we can launch the Loft command. We can go ahead and follow the exact same steps we followed in the last movie, by clicking Add to sections, selecting the first profile, the second profile, and the third profile.
At this point, the shape looks exactly like the previous movie, because up to this point we haven't included the rails and all the selections have been the same. We're now ready to go ahead and add the rail. What we need to do is move to the rail section of the dialog box and click the Click to add button. And now it's asking us to select a sketch. And we're going to go ahead and left click on the rail and you'll notice the preview goes away. This is because of the reference geometry and this is what I wanted you to see. If we were to go ahead and select OK here you'll see that we get a failure, and if we expand that failure all the way down to where we get all the information, it says the attempted Loft operation found a rail curve intersecting a section more than one time, okay.
Let's cancel this and take a look. What is happening is, Inventor selects this rail and it follows it up until it finds this intersection point and then because this is reference geometry it continues and follows this and it says that this is intersecting multiple times, because it's a single loop. To fix this, we can go ahead and add a sketch for the rail sketch. We're going to go ahead and double click on that and return to an isometric view by clicking the home button in the view cube. And now all we have to do is select each of the reference lines, right click, and then select Construction.
Again, left click, right click, Construction. By doing this, what you're doing is telling Inventor that this truly is Construction geometry. The only reason it's there is we needed an endpoint that intersected that profile. We don't want Inventor to look at it when the Loft is being created. By converting to Construction geometry, that's exactly what'll happen. Let's go ahead and finish the sketch and return to the Loft tool. We'll go ahead and repeat the process, we'll select each sketch, which gives us the preview that we saw before, now we're going to go ahead and click in the rail section, and we're going to go ahead and click the rail on the right side.
Now if we rotate to the front view, you can see something interesting happen, and this is why we needed both rails and we needed it mirrored. When we selected the first rail, Inventor did exactly what we told it to, it made the 3D shape follow this rail, but at the same time as it bowed out on this side, it pulled the model on the other side as well. This is easy to resolve by adding another rail. We'll go ahead and click in the rail section, and then we'll left click on the rail on the opposite side. And now you can see both rails control the shape of the 3D model as it transitions through each profile.
If we go ahead and select OK and hit the home button, you can see our model. The beauty here is that because this is a parametric model, and we have a unique sketch for those rails, we can always go back and make modifications. If we return to the Loft in the browser and click the plus symbol next to it, you'll see that we have Sketch1, Sketch2, Sketch3, and Sketch4. Now from time to time, I may rename the sketch. As a matter of fact, if you left click once and then left click again on the name of the sketch, you can simply type new information here.
I'm going to go ahead and add the word rail at the end. This doesn't affect the feature at all, it just makes it a little bit easier to see that this is the sketch that holds the rails when you need to make edits. If we double click on that, we return to the sketch that we just created, and here we can left click and drag on either of the rails, and because the symmetry constraints are enabled, we can make modifications on both sides equally. Once we've made some modifications, if we finish that sketch, you can see that the rails completely update and change the shape of this model based on those spline rails.
This should give you incredible control over the actual 3D shape of your model.
- Reviewing interface changes
- Projecting and importing geometry
- Working with Autodesk AnyCAD
- Understanding part modeling
- Building parts with placed features
- Working with partial chamfers