Join Thom Tremblay for an in-depth discussion in this video Advanced modeling 2, part of Cert Prep: Autodesk Inventor Certified Professional.
- [Narrator] This will be lesson two of three for Advanced Modeling Certification Objectives. For this lesson, I'll focus on creating a multibody part, as well as using surfaces to develop a part. I'll begin by completing the design of my upper housing. Part of my housing is presently a T spine body represented as a surface. I can modify the form of this by making an edit and using the edit form tool.
I'll grab two top edges, and make a simple modification to the shape, and then return back to my solid modeling environment. The hybrid modeling environment inside of Inventor allows you to be very creative by mixing a combination of T spine bodies, traditional surfaces, and solid models to define your geometry. This makes it very easy to develop essentially any shape that you can imagine. One of the things I'd like to do is use this contour as the definition of the path that will draw oil up out of the pump, or release oil out of the pump.
So I need to add a thickness to this or second shape to it. I'll use the Thicken/Offset tool, and I can use the tool to just simply add solid geometry to it. Instead, I'll use it to add surface geometry to it. And I'll set an offset value, defining the thickness of the wall, and click OK. In this case, there has to be a mathematical adjustment because of the contours of the original shape, but it's certainly something that's going to be within tolerance of the manufacturing process anyway.
The only other thing that I need is I need a work feature to create a face across this physical face. So this is one of those situations where having a physical face won't give you all of the tools that you need. So I need to create a plane. I could simply select this plane and drag a distance off of it, or tell it to be coincident, or I can use a different technique, which is selecting three points on that plane. I could also select two axes and construct the work plane in that fashion.
Now I'll use the sculpt tool, which is in the surface panel. I'll tell it that I want to use this plane and my two surfaces. You'll see these icons appear: a ball with an arrow on either end. I can use this to define which side that I want to work with. For example, the ball on the inside surface I'll point outward, and on the outside surface, I'll point inward.
I'll go back to making that neutral, and it's showing me that it will develop a solid around that face. And I can see through the hole that it is indeed hollow. However, it does not go down into the lower section. It doesn't create an opening at the bottom. I can fix this. I'll turn visibility of the work plane back on, and I'll also turn the invisibility of the original form back on.
Now I can use the sculpt tool again, select the plane, and select the surface, telling it that I'd like to cut. And it detects what I can cut, and creates the opening up into the body. Switch my visibilities back off, and I've got my part pretty well defined. Now I'd like to take this to another level, I'll switch to a different part file, where I already have a body that was defined again using a form.
In this case the entire body is defined using a form, and what I want to do is make sure that I can create a parted file, a plastic part that will separate properly. First, I'm gonna go ahead and define a 3D sketch. And I'll tell it that I'd like to create a silhouette curve of this body using the Y axis of the part.
When I do this, it follows the sharp edges very nicely, but here it appears that my sharp edge is tucked inside of the model. So I need to make a modification there. I'll finish my sketch, I'll edit the form, and again use the edit form tool, select an edge, drag it out a bit. That looks like that will resolve the problem.
I'll finish the free-form modeling tool, and now I've got my sketch. The reason I need to create this sketch is I wanna create a surface based on it in order to split my part, but I also want my part to be hollow. The shell tool can be used for many things. It can be used to remove a face and make a body hollow. It can be used to remove a face, adding a thickness to make a body hollow. In fact, I'll just show you a quick example of each of those.
I'll just quickly create a shape, extrude this out, and use the shell tool in a more traditional fashion, where I can select faces that I'd like to remove, I can change the thickness. I can use an override to tell it that certain faces have a higher thickness.
So I'll make that wall thicker than the others. Or, I can do what I want to do with this model. With this model, what I want to do is use the shell tool without selecting a face. Set the value, and what it will do is, in essence, it will hollow out my part. With my part hollowed out, I can use the rule surface tool, select my 3D sketch, reverse the direction of my ruled surface, and set a thickness value.
When I click OK, I now have a surface that I can use to split my part. I'll start the split tool, tell it that I'd like to split the solid. Select my surface, and generate my new solid, which is in fact now two solids. In the browser, I now have a folder called solid bodies that has two solid bodies within it. Solid body two is the bottom, solid body three is the top.
I'll turn off the visibility of solid body three. I can see that inside it's hollow, set to the thickness that I desired. I'll turn off my ruled surface, just for clarity, and I've got a lip that goes all the way around. If I go back to my form and make a modification, for example, taking this top edge and raising it up, when I finish my free form and turn solid body three back on, you'll see it is drawn much higher than it was.
- Certification tips
- Working with project files
- Modeling parts
- Advanced modeling features
- Designing with sheet metal
- Controlling assemblies
- Applying weldments
- Building presentation files
- Editing drawings and views