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Finalizing main body design

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3D Model Creation with Autodesk Fusion 360

4.7（148 個評分） | 3.4K 名學生已註冊

課程 3（共 5 門，CAD and Digital Manufacturing 專項課程）

Design is the first phase in the digital manufacturing process. In this course, through a series of lectures and hands-on lessons, we’ll examine a designer’s approach to the design and manufacturing process—from concept to 3D model. We’ll start by applying design thinking to understand user needs, and then we’ll explore design criteria as we dive deeper into Autodesk® Fusion 360™ sketching, modeling, rendering, and documentation features.

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4.7（148 個評分）

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JM

Dec 04, 2018

Simplemente, Excelente! Sencillo de aprender pero un reto si te propones a sacarle el máximo provecho.

VB

Jan 24, 2019

Good course to know about design process with example

從本節課中

2D Sketches to 3D Solid Model

This week expands on our layout sketches and begins to create a solid 3D model. Through the use of some basic and advanced features, we learn various tools of the trade to create complex 3D shapes. We also expand our Autodesk® Fusion 360™ knowledge and skills into the Patch workspace and explore how to add or remove solid geometry with surfaces.

Creating motor mounts8:39

Inserting motors and props8:04

Smoothing body reliefs5:49

Removing unwanted mass9:47

Finalizing main body design7:05

教學方

Autodesk Education

腳本

In this lesson, we'll be finalizing the main body design.

After completing this lesson, you'll be able to create a fillet, create a mirror,

and combine bodies.

The last step that we want to do to the extrude cuts that we've created is to make

sure that we have rounded corners.

All right, because we already rounded the corners on the overall body before

we did the extrudes and the offsets, most of the corners are already taken care of.

Some of these we're going to leave square like these edges right here,

just because we can deal with them later once we combine a left and

a right hand side of the body together.

But we do need to take care of the corners where the motors meet and

in these edges here.

So we're going to use F on the keyboard, and

the edges that we want to start with are all the ones around the motor.

So just come in, select all these edges.

And then we can come into these corners as well.

We will also have to select the other motor, so

we'll have to manually move over to this section, and we'll grab these.

And an instance where, again, we could use Rule Fillet,

we could use Rule Fillet here.

But one of the things that I don’t like about Rule Fillet in this instance is

that it'll also grab this internal bottom edge and round that.

And while that might be great,

I don't want that to be the same radius as what we're doing here.

So let's start out with a 2 mm radius and see if it'll allow this.

So everything looks pretty good, we could go a little bit bigger.

And 3 mm is probably going to be about the limit in this smaller section here.

And you will notice that it doesn't like it in this corner,

it's leaving a sharp edge there.

If we take it back down to 2 mm, it doesn't like that either.

So what's happening here is if I hold down the Control key and

we take a look at this, there's actually a slight section that curves away here.

And this fillet is large enough to encompass that.

So what we could do is we could adjust the cut so that we take a tangent line out and

completely get rid of that.

Or we can come back after the fact and

add a secondary fillet since it goes up to that sharp edge.

And we'll have to do this on both sides as well.

And if we add 3 mm here, it should round that corner out just fine.

And that does happen from time to time, especially if your curvature is

changing and the fillet completely removes one of those faces.

Oftentimes, you'll see it'll go to a sharp corner.

So we'll say okay there as well.

And let's flip this over and let's take care of the bottom.

So we're going to do a fillet, and again, this time we're going to come into these

areas, and we'll likely use the same diameter, same radius value.

But we will have that same problem down here,

where it's going to remove that face completely.

So we'll have to keep that in mind as we go through this process.

And again one of the benefits here,

it's nice because we already rounded the corners on all the cutouts.

So we don't have to worry about doing every edge on this fillet.

If you change the way that you do the design process and

you make this cutout while everything has square edges on them or

sharp corners, then you will have to select a lot more edges for your fillet.

Let's come over here, and let's finish up this process.

Now, one thing about the cutouts that we made and

basically the areas that we're talking about here,

these are structural improvements because we have this I-beam shape.

And the I-beam shape is very strong in certain directions and

not as strong in other directions.

So what we're doing here is we're actually reducing the weight, but

we're keeping it pretty much the same strength.

I say pretty much because we won't really know until we do an analysis of it.

But we're keeping it fairly strong by reducing a good amount of weight.

So this is a great way,

especially with a quad copper design, to actually reduce the weight.

Now we do need to keep some of that structure in the middle.

And we do need to make sure that we are aware of the forces that go on here, but

what we're actually going to end up doing is we're going to have the engineer go

through and perform a simulation on this.

So that way, we have a good idea of what's actually happening.

And then we'll know for sure whether or not we need to make any changes.

All right, so this one here seems to have done okay with the fillet.

It didn't completely encompass that.

But the one on the other side looks like it could use an additional fillet here, so

I'm going to add 3 mm and go ahead and say OK.

And now we've taken care of all those fillets.

You could do some additional work,

like rounding these corners off, making a small chain for there, and as I mentioned,

we could cut out some more material here if we wanted to.

But as of right now, I think everything looks okay.

I'm going to flip this back around.

We're going to go to a top view.

We're going to fit it to screen.

And I think I want to go ahead and apply a mirror at this time as well.

So under Create, we're going to mirror this body.

We're going to mirror it across the right plane.

And then we're going to come into Modify > Combine.

And we're going to join these two together.

So now in our Bodies folder, we have a single body for all of the solids.

And we do have some surfaces here.

We do have some additional cuts, things that we can get rid of.

I'm going to go ahead and actually right click on both of those and remove them.

But I want to leave Body Top, Body Bottom, and the copy.

I want to leave those in there because I'm going to need them.

Now, I'm going to rename Body 10 to be XStar Body.

So at this point, we've done most of the overall shape design work.

We started by laying out the front shape.

And we laid out the top shape, and we used those two sketches to build this in 3D.

Now as I mentioned initially, we kept the front shape fairly simple.

As we look at this, it's really just an arc, and

the reason we did that was to simplify the design process a little bit.

Now that doesn't mean that you have to do that every time you make a design in 3D.

You could certainly create curvature in three dimensions, but

since we were looking at this overall design, keeping it symmetric,

it made more sense to keep that front shape the same.

So everything here looks pretty good.

We have a lot of areas that we can still add material to or

actually work on the structure of.

And we're going to take a look at that in the next lesson, but for

right now, everything looks good, so we want to make sure that we save our file.

That way we can move on to the next step.

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