Create solids from sketches

00:02

Create solids from sketches.

00:05

After completing this video, you'll be able to

00:07

create an extrude, a revolve a loft and a sweep

00:12

in fusion 3 60. We want to begin with the supply data set. Create solids dot F 3D.

00:18

Make sure that you do upload this to your

00:20

data panel in whichever project and sub folder,

00:22

you're storing your data sets in

00:24

this create solids design has several sketches under the sketches folder.

00:29

We have extrude revolve loft as well as sweep

00:33

to get started.

00:34

We want to begin by hiding our sweet profiles

00:36

and showing the first sketch called ex shrewd.

00:39

When we create an extrude,

00:41

we need to have a closed profile and this rectangle

00:44

fits that you can see we can preselect the area

00:48

and then select extrude.

00:50

Once we select extrude,

00:51

we can begin pulling this up into 3D or using

00:54

the onscreen manipulator to change the draft or taper angle.

00:59

This is a quick way for us to generate a solid body by using a closed profile.

01:05

We're going to create a new body and say, OK.

01:08

Now in the body folder, we have body one, we're gonna rename this to be extrude.

01:14

We're gonna hide the extrude. And next, we want to show the thin extrude sketch

01:19

this time, let's select extrude and note that in the type section,

01:22

we have extrude and thin extrude.

01:25

Now, even though we're in these solid tools,

01:27

the thin extrude is an option when we have an open profile.

01:31

If we zoom in, you can see here that we're able to create an extrude

01:35

using not only the height or distance but also the wall thickness,

01:40

we can change the wall thickness. In this case, let's set it to three millimeters,

01:43

determine which side we want or if it's centered on our sketch and we can say, OK,

01:48

and create a new solid body.

01:50

Note that when you're creating a new solid body,

01:53

if multiple bodies are displayed fusion will default to joining them together.

01:58

So make sure that you always take a look at the operations. And if you want new bodies,

02:02

you want to join them together or remove them

02:04

from other solids that you use the applicable options.

02:08

Next, we want to take a look at creating a revolve.

02:11

Revolve is another way for us to use a closed profile to generate solid objects.

02:17

With the revolve,

02:18

we're gonna be taking a closed profile and spinning it around an axis of revolution.

02:23

The revolve sketch used the center line option which made it pres

02:27

selected as the axis of revolution.

02:29

This is a great way to create complex shapes that

02:32

are revolved about an axis with a single sketch.

02:36

Once again, we're going to create a new body.

02:38

But let's take a quick second to note the options that we have.

02:41

We have a partial option which allows us to determine how far we want to revolve.

02:46

We can also do to another object.

02:48

If we had another solid object,

02:50

we wanted it to stop at or a full 360 degree revolution.

02:54

For this example, I'm gonna do a partial of 100 and 80 degrees.

02:58

So we can see inside of that revolve.

03:01

I'm gonna rename each of these, then extrude for body two

03:06

and body three. We're gonna name revolve.

03:10

Let's hide the revolve and let's move on

03:12

to creating something a little bit more complex.

03:14

And that's gonna be a loft.

03:16

We've got loft 12 and three and we have loft rails.

03:20

When we're creating a solid loft, we still need to have two D closed profiles.

03:24

But we could also use the selection of a planar face

03:28

with each of these.

03:29

What we're going to be doing is generating

03:30

a shape that goes through each of these profiles

03:34

to get started. We're gonna go to our create menu and select the loft tool

03:38

in the top section.

03:39

We wanna have our profiles which are gonna be each of these three closed sections.

03:44

As we do that, we can see a solid being generated on the screen.

03:48

We do have some control over the start and end profiles.

03:52

If we were using, for example, a selected face, we could drive tangy

03:56

based on that selection

03:58

for our purposes.

03:59

However, we're going to go down to the rail section, we're going to hit the plus icon

04:03

and we're gonna add rails,

04:05

we'll hit plus again and we'll add a secondary rail.

04:09

If we view this from the top,

04:10

the loft is going to follow the shape of those rails

04:13

using multiple profiles and rails can be a

04:16

tricky thing for getting good quality outcomes.

04:19

So you need to be careful that you're not over defining your shapes.

04:23

For example,

04:24

we might determine that profile two isn't needed because

04:27

when we look at it from the front,

04:28

we can see that there is a slight bulge that happens here,

04:32

we can select and remove that profile and the

04:35

final result is going to be a much smoother transition

04:38

without driving that middle profile shape.

04:41

So keep in mind as you begin defining more

04:44

complex designs that you want to be careful,

04:47

you're not over defining the inputs.

04:49

In

04:49

this case, we're going to say, OK, with just the start and the end profile,

04:53

we'll hide the sketch loft two and we'll rename body four.

04:57

Let's go ahead and hide that and take a look at our last example, which is a sweep

05:02

for this. We have a suite profile and we have a path as well as a guide rail.

05:07

We're going to go to our create menu and select suite.

05:11

There are a couple of different ways we can create a sweep.

05:14

We can use just a single path, a path and a guide rail or a path and a guide surface.

05:19

We're not going to be looking at the guide surface option here,

05:22

but this is a great way to define the direction

05:25

of your profile as it sweeps around a path.

05:28

We're going to start with a single path option by first

05:30

selecting the profile and then grabbing the center line path.

05:35

When we view this from the top, we can get an idea of the shape that's being created.

05:39

If we change the option to be a path plus guide rail,

05:43

the guide rail is going to be this secondary edge.

05:46

We can see how that's changing the sweep profile

05:49

as we go along the guide rail and we go along the guide path.

05:53

We're now making the shape larger as it progresses through that distance.

05:58

We also have control over how far this goes along our path.

06:02

And whether or not we use profile scaling

06:05

right now, it's scaling based on that section.

06:08

We can also have it stretch which would keep it the same height as the original,

06:12

but it would make the outsides stretch as it goes through.

06:15

And we can change whether or not this is perpendicular to the path

06:19

or if we want it to twist as it goes.

06:21

Because the guide path and the guide rail are both planar this

06:25

is not going to have any effect on our current design.

06:28

But keep in mind that it's important that we explore all

06:30

these options to determine which one fits best with your design.

06:35

Now that each of these shapes has been created,

06:37

we could also continue on using additional creation tools,

06:40

things like mirror to mirror a body.

06:43

And we can use the bottom face or planar face

06:47

and we can create a single blended pipe section

06:51

just by simply using those basic inputs and then additional tools to modify it.

06:59

Let's go ahead and rename this sweep

07:01

and make sure that we do save the design before we move on.