Join John Helfen for an in-depth discussion in this video Creating complex shapes with the Loft tool, part of Inventor 2014 Essential Training.
We're now to a point where we can take all the things we've learned and work on one of the more complex sketch features in Inventor, and that's called the loft. On the screen you can see a basic maybe shampoo or salad dressing bottle shape that we're going to create through out this video. A loft is essentially a 3D model that transitions through a series of shapes. And the shapes don't have to be the same. In this case I'm using a couple of ellipses and a circle. But it could be a square, it could be any shape you draw.
The more complex the sketches get, the more time it's going to take to ensure that your loft is being created properly, but in general, you should be able to transition from a bunch of different shapes. To work through this, we're going to create a new part file. I'll select New from the menu. I'll select Standard.ipt as my template and click Create to begin the new part file. To start, we need to create our very first sketch. And to do that, I'll create a 2D sketch, and select the x z plane to sketch on.
Now we're creating the bottom of the bottle here, so what I want to do is use the ellipse tool to create my initial ellipse shape. Now that I have the basic shape, I'm going to dimension. I'm going to set the overall width from center to be, let's do 1.5. I'll hit Enter on my keyboard to enter that value. And then I'll do the overall height or width of the bottle to be, let's say 0.75. That gives me the basic shape I'm going to use as the bottom of this bottle.
I can finish this sketch and I'm ready to continue on. But before I do that, what I want to do is go back to the origin geometry folder, click the plus symbol and find the xz plane and right-click on it and select Visibility. I just want this available because I'm going to use this to create the additional workplanes needed to create the additional two profiles we're going to use. While learning about work planes, we earned about a shortcut where we can create offset work planes from within the 2D sketch command, and we're going to use that right now.
I'm going to create a new 2D sketch, but instead of left-clicking on this plane and sketching on the plane we just used, I'm going to left-click and drag, from that plane, and enter a value of three. When I hit Enter, the work plane is created and the sketch is automatically generated on that work plane. Next I'm going to return to the ellipse tool. I'm going to start from the center point and drag out to the left. And this time I, I'm going to go a little bit further past the outside of this original sketch that I see below.
And, a little bit wider than that as well. I'll right-click and select General Dimension from the marking menu, and I can add some dimensions here. The overall width from center I'm going to set to 1.75 and hit Enter on my keyboard, and then I'll do an additional dimension on the outer edge. At 0.8 inches. I'm now ready to finish this sketch. And you can see that I have two profiles now created for this loft. And I have one left to create.
So, I'm going to create a new 2D sketch one more time. And we will create an offset work plane by left-clicking and dragging from the existing work plane. And I'll enter a value of two inches. The work plane is created, you can see them all here in the browser, and I'm in Sketch3 on that plane now. To finish up, I'm going to right-click in the graphics window and select Center Point Circle. I'll start from the center of the sketch and I'll enter a value of one, and hit Enter on my keyboard. I'm now ready to finish this sketch and I have all the profiles needed for my loft.
The loft tool can be found in the Create panel on the 3D Model tab. When you click on the loft command, you're entered into the loft dialogue box, and just like extrude and revolve, you have a lot of the same options You do have the ability to create a new solid. If this weren't the base feature, you could create joins, cuts and intersects as well. But because this is the base feature, it's always going to be a new solid. I also have the ability to create solids or surfaces, but we're going to stick with a solid model. And we have the ability to begin selecting sections we're going to loft through.
I'm going to click to add a new section, and I'm going to start with the base of the bottle. Since there's only one profile, Inventor automatically selects the entire profile. I can then add an additional option by either clicking add, or I can simply go and click on the next shape and it's automatically added to the sections dialogue. And you can start to see the transition happening. Finally we'll select the final item and you can start to see the overall shape within the preview.
You can see our model bows out a little bit on the side and works its way back to the circle. Same on the outside as well. It's going to bow out. It's going to transition through that point, or through that profile. And up to this circular profile. Now, we could add rails to control this, and we'll do that in the next video. But I wanted to touch on the Conditions tab. The Conditions tab is another way to control the overall shape of this bottle without having to create rails.
And it's not quite as accurate as rails. You'll see in the next video. But it does provide a lot of flexibility to tweak or adjust how the shape of the bottle looks. In general, without having to go through the additional steps of creating rails. In the Conditions tab, we have the ability to change from what is a Free Condition where Inventor naturally just follows its own natural free form through the shapes, to a Direction Condition. By doing that, we enable the Angle in Weight options in this tab.
And if we zoom in, we're looking at section one, which is this bottom section. And if I zoom in, you'll see that we are 90 degrees from this horizontal line, up and to the right. So this sketch starts out 90 degrees from horizontal and it begins to move towards the next section. If we wanted to change that, we could set from 90. We could set it to, let's say 15. And you can see that it works in before it starts to transition to the next profile.
And we can adjust the weight here to two, and you can see it essentially pushes how long this follows that 15 degree angle before it begins transitioning. If we set this to four, you can see that it pushes much, much further toward the center of the model. Let's go ahead and set it back to a weight of two, and let's set this, instead of 15 degrees, let's set it to 120 degrees. With 120 degrees, it's going to start moving outward first before it transitions.
If we zoom out you can see the results of making those changes. The other thing to keep in mind is that it doesn't just happen from one side. It happens from all directions. So, it is bowing it in multiple directions, which is another reason you might want to consider lofting along rails depending on how accurate you need your model to be. You know, how much control you want over the shape of the bottle. If we rotate back to the front-view, and zoom in a little bit on the top of the bottle, you can see the result of changing to a direction condition on the neck.
Here we want it to be 90 degrees coming down from this sketch but I'm going to increase the weight so that you can see how we can add a neck shape to this. As I bump that up from one to two to three, let's even go to five. You can see that I can control how the shape of the bottle looks as it transitions through these items. I'm go ahead and set these back to their default conditions so that we can hit okay, and complete this portion of the course.
Essentially, we've used all that we've learned through work features, through sketching, and through part modeling to create a basic shape of a bottle here.
The course was created and produced by John Helfen. We're honored to host this training in our library.
- Customizing Inventor's menus
- Drawing rectangles, arcs, splines, and slots
- Moving, copying, and rotating geometry
- Trimming, splitting, scaling, and stretching geometry
- Creating work planes
- Projecting and importing geometry
- Creating extrusions, revolves, sweeps, and lofts
- Adding holes to a part model
- Creating rectangular feature patterns
- Creating iParts and iFeatures
- Using constraints to position parts
- Creating drawing views
- Setting dimensions