Join John Helfen for an in-depth discussion in this video Complex shapes with the loft tool, part of Autodesk Inventor 2018 Essential Training.
- [Voiceover] We're now ready to look at one of the more powerful part modeling features, and that's the Loft command. On the screen, you can see a bottle I've created, and we're gonna recreate that using the Loft command, and at this point we're also gonna include a lot of the other things we've learned up to this point in the course, such as creating different sketches and work features. To begin, we're gonna need a new part file. I have one opened down at the bottom of the screen. If you don't have one, go ahead and start a new part file, and we'll begin by creating a new sketch. We'll right click and select New Sketch, and we'll select the X-Z plane to sketch on.
To begin, we're gonna need to create an elliptical shape to make the base of the bottle. To do that, we can go to the Sketch tab under the Create panel, and select the arrow underneath Circle, which will expose the other options, one of which is Ellipse, here at the bottom. We'll go ahead and left click on the center of the sketch and drag to the right, and we'll left click to place our first point on our ellipse, and then we'll drag our cursor up above the center of the sketch, and we'll left click to create the final ellipse.
Next we're gonna add some dimensions. To do this, we'll right click and select general dimension, and we'll select our ellipse and drag upward. This will allow us to enter this dimension. We'll enter 1.5 here, and hit Enter. Next, we'll repeat that process, but instead of dragging up, we'll drag out to the right. Here we'll enter .75 and hit Enter. We now have the ellipse that will be the base of our model. We can click Finish Sketch, and zoom out a bit, and as you remember, when we first created this ellipse, we started sketching on one of the origin planes, and I wanna turn that origin plane on because I'm gonna use it to create other work geometry that we can create other sketches on.
So we're gonna go to the browser and click the plus symbol next to the origin, and I'm gonna find the X-Z plane. If you selected a different one, go ahead and find it and right click on it, and select Visibility. What you'll find is you now see the work plane, the X-Z plane, visible in the graphics window, and if you've watched the work plane movie, you'll remember that we do have a shortcut for creating offset work planes, and that is to create a sketch. Within the Sketch command, you can create offset work planes very easily, and that's what we're gonna do here to create the additional two work planes and two sketches we need for this loft.
To do that we're gonna right click, select New Sketch, and instead of simply left clicking on a work plane to select it, we're gonna left click and hold the mouse button down and drag upward with our mouse. You can see we're now creating an offset work plane, and we're gonna enter a value of three and click the green check mark. By doing that, the new work plane is created, work plane one, and a new sketch is created on that work plane. Now we're gonna create the ellipse that's gonna make the middle of the bottle. We can return to the create panel and select Ellipse again.
Left click on the center of the sketch and repeat the process, this time dragging a little further to the right than the previous ellipse, and a little bit higher than the previous ellipse as well. Now we can go ahead and add the dimensions, we'll right click and select General Dimension. Left click on our ellipse and drag upward, and left click to place our dimension. Here we're gonna enter 1.75 and hit Enter on our keyboard, and we're still in the Dimension command, so we'll go ahead and left click the ellipse one more time.
This time, rather than dragging up, we'll drag out to the right, and we'll enter .8 for that value. We've now finished our second sketch, we can finish that sketch by left clicking Finish Sketch in the ribbon bar. And we have one more sketch to create. Let's right click, select New Sketch. This time we'll left click and drag on work plane one. We'll drag it upward, and we'll enter a value of two for the offset distance. Clicking the green checkmark creates the work plane, and it enters us into that sketch.
Rather than creating a third ellipse, this time let's right click and select Center Point Circle. This will be the top of the bottle. We'll left click at the center of the sketch and enter a value of one on the heads up display, and then hit Enter on the keyboard to create our geometry. We now have all three sketches, so we can finish this sketch, and we're ready to create the Loft feature itself. To do that, we can go to the 3D Model tab under the Create panel and select the Loft command. Now, when you see this dialogue box, it should immediately become somewhat familiar to you.
Some of the features that we've already learned about in Extrude and Revolve are present here as well. On the left-hand side you can see we have New Solid, because this is our fist base feature, we don't have the options for Join, Cut or Intersect. If this were the third, fourth, or fifth feature, these would be available to us. Down below that you can see we have the two different types of output of solid or surface, and we'll leave it at solid. Over on the right, you see the rail section of the dialogue box, and we'll look at that in the next movie. The area we wanna focus on now is this Sections area.
In that area, you can see Click to Add. If we were to click here, we would get some feedback that says, "select a sketch". We can start by selecting sketch one, and you can see that's been updated to include sketch one. Instead of clicking to add up here, we could also simply select the sketch, and you can see it's automatically added to the sections. You can also see a preview being generated. Right now we only have two profiles selected, so you see a preview of what the solid would look like if we were to simply hit Okay here.
But we're not quite finished. We wanna add this circle at the top as well, and if we left click on it, the profile updates to reflect that change. Let's go ahead and click Okay, and we now have our completed loft. If you look in the browser, we have the loft one feature, and if you click the plus symbol next to it, you can see that sketch one, sketch two, and sketch three have been consumed by that loft. While we're in the browser, let's right click on the Loft feature and select Edit Feature. This'll place us back into the dialogue box, and the reason I want to jump back here is I want to take a minute to look at the Conditions tab.
This is another way that you can control the overall shape of the 3D model based on some basic settings. Let's take a look. I'm gonna rotate to the right side view, and I'm gonna zoom in to the bottom near sketch one. And the reason for this is, as we make changes in the dialogue box, this preview is gonna update, and it's gonna help to see that. By default, the initial condition for all sections is gonna be a free condition. If we select the dropdown next to sketch one, we also have another option for direction condition.
By selecting that, you'll see the preview updates, because now the angle and weight options are available, and Inventor is using those to evaluate how this shape should be created. For example, if we were to change this 90 degree angle to 30 degrees, you'll see that, rather than starting right from this profile and going straight up 90 degrees, it's coming in at a 30 degree angle with a weight of one. Now, what is a weight of one? It's actually just a proportion.
Right now, this is one, but we can increase that to, say, two, and you can see that that weight is much more pronounced. Essentially, what it means is it moves much further inward before it begins to make the transition to the next profile. I'm gonna go ahead and return that to one. Let's go ahead and change this from 30 degrees to 120 degrees. Now one thing I'll mention is you do want to make sure this degree option is there as well. That text is helpful. Now with that change you can see the 120 degrees now moves outward before it starts moving up.
And we're gonna go ahead and leave the weight at one. Next, let's zoom out and move up toward sketch three and use the condition settings to create a neck on this bottle. Rather than the free condition for sketch three, let's click the dropdown arrow and set it to direction condition. We'll go ahead and leave this as 90 degrees, we want this to start at a 90 degree angle, what we want is it to go further down or have a wait time or a wait before it starts to transition.
What we can do is simply start increasing the weight from one to two. Let's make it three. Go ahead and hit backspace and make it up to five. And what you can see is it takes a much longer time before it starts to transition through that next profile. We'll click Okay, and now, if we hit the Home view, you can see we have a much different shape than what we started with just by modifying the condition options.
- Reviewing interface changes
- Projecting and importing geometry
- Working with Autodesk AnyCAD
- Understanding part modeling
- Building parts with placed features
- Working with partial chamfers