Create a 3D mechanical link

00:02

Create a three d. mechanical link.

00:05

After completing this video, you'll be able to

00:08

disable, capture design history,

00:09

create a fully defined sketch and use extrude and fill it.

00:14

Infusion 3 60. Let's get started with the supply data set D.

00:17

Feature link dot F three D.

00:20

In most cases when you upload an F three D.

00:22

To fusion 3 60 it contains history of how the part was created. In some cases in F.

00:27

Three D. Can be created but not contain any history now.

00:31

This imported model doesn't contain any sketch

00:33

or feature history that can be manipulated.

00:35

We want to create a full featured parametric model of this link

00:39

and there are a couple ways that we can do this first.

00:42

Let's talk about capturing design history and what that actually means.

00:46

Infusion 3 60 anytime we create a sketch of feature or

00:49

any of the other tools used in fusion 3 60 history is

00:53

maintained meaning that there is an order of operations to create that

00:56

part and something that we can go back to to manipulate.

00:60

In a case like this, we have an F. Three D file that doesn't contain that history

01:04

in order to create it.

01:05

We can use this as a reference but we need

01:06

to be careful not to project references from this design.

01:10

Otherwise we will contain links between the two and really

01:14

what we want is a fully featured dimension model.

01:16

So to get started,

01:18

I want to talk about capturing design history and how we can turn that on and off.

01:22

First. Let's take a look at the create menu and notice at the very bottom.

01:26

The last two options are creating a PCB and creating a base feature.

01:30

Next let's go to the gear icon in the bottom right of fusion 360 and turn on.

01:35

Do not capture design history.

01:37

We're going to select continue and if you

01:39

have a design that contains sketches and features,

01:42

all history will be removed.

01:44

Now the reason that this is important is because there are some tools that

01:47

are enabled once history has been turned off for example under the create menu.

01:52

Now we can see find features and fluid volume.

01:55

These tools are available in other areas of fusion 3 60 such

01:59

as when you're simplifying a geometric design for use with things like

02:03

generative design or simulation.

02:05

But for right now if we select find features

02:08

we expand our crank arm component

02:10

and we select the body.

02:12

We can have it look for things like patterns, mirrors revolves extrude and champers

02:17

we say okay

02:19

it creates a history in the browser.

02:21

It lets us know how it thinks this part was created.

02:24

Notice that there are a lot of extrude revolves.

02:27

There's a mirror of certain geometry.

02:29

You can see here that these occurrences are the text on the other side of the link.

02:33

Also note that there are a lot of filets.

02:35

These filets are contained on a lot of the text

02:38

as well as in certain areas of the model.

02:41

Now even though we have this history in the browser not everything can be changed.

02:46

Some things can be edited. Things like filets.

02:48

However, if we select an extrude and right click there's no edit option.

02:53

So another thing that we can do when history is

02:55

turned off is we can manually de feature this part.

02:58

If it helps us reverse engineer it.

03:00

For example if we want to get rid of the recesses and

03:03

the text we can select these inside faces holding down the shift key

03:08

and then we can go to modify and delete

03:11

Fusion 3 60 is able to patch and reconcile the

03:14

geometry around this area by simply removing those faces.

03:18

You can also use delete on the keyboard to make that happen.

03:22

Other areas of the design such as these filets can be removed as well. If we wish

03:27

for example we can select the filets on this end and hit delete

03:32

once we're done removing features from apart to

03:35

help us reverse engineer it we can always

03:37

go back to the top level of our browser right click and capture design history.

03:42

This will create a new component and base feature for the crank arm but

03:46

any of the history that was used to remove certain features has been erased.

03:51

So at this point in time it's important to note that this crank arm

03:54

is a component and when starting new designs in fusion 3 60 in general,

03:59

it's a good idea to create a new

04:00

component components are required for mechanical motion.

04:04

They ease when you're creating exploded views and animations

04:07

and they also help downstream when creating detailed drawings.

04:10

They also will aid an organization of your timeline and your browser.

04:15

So for this example let's get started by going to assemble and new component,

04:20

we're going to be creating a new component called link

04:24

and will simply hit enter

04:26

the new component is created which contains its own coordinate system.

04:30

If we take a look at this,

04:31

you can see that the coordinate system is placed well above the current link.

04:35

And if we view this from the front we can actually see that the crank arm is at an angle.

04:40

Remember that we don't want to project any references

04:43

from the crank arm into our new link.

04:45

So we're just going to be using it for measurement values.

04:48

I'm going to rotate this around and just make quick note of inspection values.

04:53

We have 10.2 millim diameter on the big end and we have a distance of 49.637.

05:01

Notice that this is a straight line distance. If we want to get an accurate distance.

05:05

It's a good idea to select the boars and we can get a distance between this.

05:10

We can also add comments to the design.

05:12

For example, 10.2 millimeter diameter big end

05:19

diameter small end.

05:22

I'm going to select post and now the comment is saved in my design.

05:26

It's a good time for you to practice using inspect and measure.

05:29

So go ahead and measure a couple other areas of the design.

05:32

For example, the distance between the top and the bottom face is 6.51 mm.

05:38

You can measure the distance between two faces here to figure

05:42

out what the distances between the opening and the closing sections.

05:46

And we can also figure out what the bore diameter is and distances for filets.

05:52

Once you've measured all those values, let's get started by creating a new sketch.

05:56

We're going to rotate this around and we're going to select the

05:59

front plane and we're going to base our design about the origin.

06:02

So using a center diameter circle,

06:05

we'll start there creating an inside and an outside diameter

06:08

and we'll do the same thing on the back.

06:11

We want to make sure that there is a horizontal vertical

06:13

constraint between the centers of each side of the link.

06:17

And then we can use our dimension tool to place

06:19

a dimension of 10.2 mm on the big end and 10

06:24

on the small end.

06:26

The outside diameter value isn't as critical, but I'm going to place this at 19 mm,

06:30

making both of these the same.

06:34

The distance between the two center points is going to

06:36

be important for the overall motion of the reciprocating saw.

06:40

In this case, I'm going to be using a value of 49.5.

06:44

Next we need to create the rectangular portion in the center

06:48

for this. I'm going to use a line from center to center.

06:51

I'm going to hit escape to get off my line tool.

06:54

I'm going to convert this to construction using my sketch palette

06:57

With it still selected. I'll use offset and I'll offset a distance of 5 mm

07:02

with the offset line. We can then use mirror

07:05

to create a mirror of that line,

07:07

selecting our horizontal construction line.

07:11

Then we want to create the flat spots on the back side of the link

07:14

for this.

07:15

I'm going to use my line tool making sure that I snapped to the outside diameter

07:19

and then use my dimension tool for the angle.

07:22

This is going to be 45 degrees overall.

07:25

So I need to make it 22 a half degrees on the one side.

07:30

Then I'll use the horizontal vertical constraint

07:32

and once more will mirror that geometry across to the other side.

07:36

Using mirror means if we make any changes to the overall design.

07:40

For example, if we decide that this angle needs to be steeper,

07:43

we can adjust it to 25° and both sides will change for this example,

07:47

we are going to stick with 22.5°.

07:51

There is one more element that we need to know and that's

07:53

going to be the diameter of the cut on the inside.

07:56

You can see that this contains a flat here.

07:59

Now we want to figure out exactly where that flat is,

08:01

it doesn't look like there's a lot of space here,

08:04

but we need to make sure that we do account for that for this.

08:07

I'm going to create another extrude. I'm going to use a small circle

08:13

and I just want to give it roughly the right size

08:18

Looking like we're gonna be at about 13 mm. This is going to be a reference for me.

08:22

So I'm going to select that and convert it to construction.

08:26

Then I want to create a vertical line that goes from the outside to outside.

08:30

And I'm going to apply a tangent constraint between it and the circle.

08:35

So this gives me the flat spot that I need.

08:37

And I can modify this dimension value,

08:39

say down to 12 or up to 14 and have

08:43

that line adjust its position figuring out these references.

08:47

It's going to be an important aspect of building a parametric design,

08:50

understanding how you want to dimension something so that it can update properly.

08:55

Next we're going to finish the sketch and we'll

08:56

be using this to create the solid body.

08:59

Well, first begin by extruding the smaller section,

09:02

I'm going to use the direction set to symmetric,

09:06

set the measurement value so that it's the full length

09:09

And this section is going to be a distance of 7.45 mm.

09:14

We'll need to expand the sketches and bring the sketch back.

09:17

We're going to exclude the other side,

09:19

making sure to include everything with the exception of these small sections.

09:23

Once again using symmetric setting it to the full length and

09:28

this side is going to be a distance of 13 mm.

09:32

We're going to right click and repeat the extrude

09:34

this time. We're going to extrude the center section.

09:37

This is going to be symmetric again the whole length and 6.5 mm.

09:43

Now we need to remove the section from the center.

09:46

Once again we can right click and repeat the

09:48

extrude and we can select the center section.

09:52

We need to hold down control or command to select multiple profiles.

09:56

Use the symmetric option the whole length one more

09:59

time and the distance between these is 4.65 mm.

10:04

Now that we've removed all of that information.

10:06

We can hide the sketch, we can hide our crank arm and we can apply some filets.

10:11

So from modify fill it.

10:13

I'm going to select the two vertical edges on the big

10:16

side and the two vertical edges on the smaller side.

10:19

And I'm going to apply a five millimeter Philip.

10:22

I'm going to right click and repeat this and apply it to the top and bottom.

10:26

This time I'm going to use the on screen manipulator and drag this out

10:30

and in this case 5.5 millimeters. And hit enter too. Okay,

10:35

so now we've recreated the link using a single sketch and

10:39

all the dimensions required as well as a handful of features.

10:42

Now we have a fully featured parametric version of this link.

10:46

We don't have the recesses or the text that was included on the original.

10:50

But all the critical features, including the hole diameters,

10:53

thicknesses and required geometry are there at this point.

10:57

Let's make sure that we do save our new link.

10:59

And instead of doing a save, I'm going to do a save as

11:03

notice that I have another folder in this case,

11:06

I want to go back and go into my parametric

11:08

modeling folder and I'm going to call this one parametric link

11:13

from here.

11:13

Continue to make any adjustments or modifications that you see fit

11:16

and then make sure that you save it before moving on.

Video transcript

00:02

Create a three d. mechanical link.

00:05

After completing this video, you'll be able to

00:08

disable, capture design history,

00:09

create a fully defined sketch and use extrude and fill it.

00:14

Infusion 3 60. Let's get started with the supply data set D.

00:17

Feature link dot F three D.

00:20

In most cases when you upload an F three D.

00:22

To fusion 3 60 it contains history of how the part was created. In some cases in F.

00:27

Three D. Can be created but not contain any history now.

00:31

This imported model doesn't contain any sketch

00:33

or feature history that can be manipulated.

00:35

We want to create a full featured parametric model of this link

00:39

and there are a couple ways that we can do this first.

00:42

Let's talk about capturing design history and what that actually means.

00:46

Infusion 3 60 anytime we create a sketch of feature or

00:49

any of the other tools used in fusion 3 60 history is

00:53

maintained meaning that there is an order of operations to create that

00:56

part and something that we can go back to to manipulate.

00:60

In a case like this, we have an F. Three D file that doesn't contain that history

01:04

in order to create it.

01:05

We can use this as a reference but we need

01:06

to be careful not to project references from this design.

01:10

Otherwise we will contain links between the two and really

01:14

what we want is a fully featured dimension model.

01:16

So to get started,

01:18

I want to talk about capturing design history and how we can turn that on and off.

01:22

First. Let's take a look at the create menu and notice at the very bottom.

01:26

The last two options are creating a PCB and creating a base feature.

01:30

Next let's go to the gear icon in the bottom right of fusion 360 and turn on.

01:35

Do not capture design history.

01:37

We're going to select continue and if you

01:39

have a design that contains sketches and features,

01:42

all history will be removed.

01:44

Now the reason that this is important is because there are some tools that

01:47

are enabled once history has been turned off for example under the create menu.

01:52

Now we can see find features and fluid volume.

01:55

These tools are available in other areas of fusion 3 60 such

01:59

as when you're simplifying a geometric design for use with things like

02:03

generative design or simulation.

02:05

But for right now if we select find features

02:08

we expand our crank arm component

02:10

and we select the body.

02:12

We can have it look for things like patterns, mirrors revolves extrude and champers

02:17

we say okay

02:19

it creates a history in the browser.

02:21

It lets us know how it thinks this part was created.

02:24

Notice that there are a lot of extrude revolves.

02:27

There's a mirror of certain geometry.

02:29

You can see here that these occurrences are the text on the other side of the link.

02:33

Also note that there are a lot of filets.

02:35

These filets are contained on a lot of the text

02:38

as well as in certain areas of the model.

02:41

Now even though we have this history in the browser not everything can be changed.

02:46

Some things can be edited. Things like filets.

02:48

However, if we select an extrude and right click there's no edit option.

02:53

So another thing that we can do when history is

02:55

turned off is we can manually de feature this part.

02:58

If it helps us reverse engineer it.

03:00

For example if we want to get rid of the recesses and

03:03

the text we can select these inside faces holding down the shift key

03:08

and then we can go to modify and delete

03:11

Fusion 3 60 is able to patch and reconcile the

03:14

geometry around this area by simply removing those faces.

03:18

You can also use delete on the keyboard to make that happen.

03:22

Other areas of the design such as these filets can be removed as well. If we wish

03:27

for example we can select the filets on this end and hit delete

03:32

once we're done removing features from apart to

03:35

help us reverse engineer it we can always

03:37

go back to the top level of our browser right click and capture design history.

03:42

This will create a new component and base feature for the crank arm but

03:46

any of the history that was used to remove certain features has been erased.

03:51

So at this point in time it's important to note that this crank arm

03:54

is a component and when starting new designs in fusion 3 60 in general,

03:59

it's a good idea to create a new

04:00

component components are required for mechanical motion.

04:04

They ease when you're creating exploded views and animations

04:07

and they also help downstream when creating detailed drawings.

04:10

They also will aid an organization of your timeline and your browser.

04:15

So for this example let's get started by going to assemble and new component,

04:20

we're going to be creating a new component called link

04:24

and will simply hit enter

04:26

the new component is created which contains its own coordinate system.

04:30

If we take a look at this,

04:31

you can see that the coordinate system is placed well above the current link.

04:35

And if we view this from the front we can actually see that the crank arm is at an angle.

04:40

Remember that we don't want to project any references

04:43

from the crank arm into our new link.

04:45

So we're just going to be using it for measurement values.

04:48

I'm going to rotate this around and just make quick note of inspection values.

04:53

We have 10.2 millim diameter on the big end and we have a distance of 49.637.

05:01

Notice that this is a straight line distance. If we want to get an accurate distance.

05:05

It's a good idea to select the boars and we can get a distance between this.

05:10

We can also add comments to the design.

05:12

For example, 10.2 millimeter diameter big end

05:19

diameter small end.

05:22

I'm going to select post and now the comment is saved in my design.

05:26

It's a good time for you to practice using inspect and measure.

05:29

So go ahead and measure a couple other areas of the design.

05:32

For example, the distance between the top and the bottom face is 6.51 mm.

05:38

You can measure the distance between two faces here to figure

05:42

out what the distances between the opening and the closing sections.

05:46

And we can also figure out what the bore diameter is and distances for filets.

05:52

Once you've measured all those values, let's get started by creating a new sketch.

05:56

We're going to rotate this around and we're going to select the

05:59

front plane and we're going to base our design about the origin.

06:02

So using a center diameter circle,

06:05

we'll start there creating an inside and an outside diameter

06:08

and we'll do the same thing on the back.

06:11

We want to make sure that there is a horizontal vertical

06:13

constraint between the centers of each side of the link.

06:17

And then we can use our dimension tool to place

06:19

a dimension of 10.2 mm on the big end and 10

06:24

on the small end.

06:26

The outside diameter value isn't as critical, but I'm going to place this at 19 mm,

06:30

making both of these the same.

06:34

The distance between the two center points is going to

06:36

be important for the overall motion of the reciprocating saw.

06:40

In this case, I'm going to be using a value of 49.5.

06:44

Next we need to create the rectangular portion in the center

06:48

for this. I'm going to use a line from center to center.

06:51

I'm going to hit escape to get off my line tool.

06:54

I'm going to convert this to construction using my sketch palette

06:57

With it still selected. I'll use offset and I'll offset a distance of 5 mm

07:02

with the offset line. We can then use mirror

07:05

to create a mirror of that line,

07:07

selecting our horizontal construction line.

07:11

Then we want to create the flat spots on the back side of the link

07:14

for this.

07:15

I'm going to use my line tool making sure that I snapped to the outside diameter

07:19

and then use my dimension tool for the angle.

07:22

This is going to be 45 degrees overall.

07:25

So I need to make it 22 a half degrees on the one side.

07:30

Then I'll use the horizontal vertical constraint

07:32

and once more will mirror that geometry across to the other side.

07:36

Using mirror means if we make any changes to the overall design.

07:40

For example, if we decide that this angle needs to be steeper,

07:43

we can adjust it to 25° and both sides will change for this example,

07:47

we are going to stick with 22.5°.

07:51

There is one more element that we need to know and that's

07:53

going to be the diameter of the cut on the inside.

07:56

You can see that this contains a flat here.

07:59

Now we want to figure out exactly where that flat is,

08:01

it doesn't look like there's a lot of space here,

08:04

but we need to make sure that we do account for that for this.

08:07

I'm going to create another extrude. I'm going to use a small circle

08:13

and I just want to give it roughly the right size

08:18

Looking like we're gonna be at about 13 mm. This is going to be a reference for me.

08:22

So I'm going to select that and convert it to construction.

08:26

Then I want to create a vertical line that goes from the outside to outside.

08:30

And I'm going to apply a tangent constraint between it and the circle.

08:35

So this gives me the flat spot that I need.

08:37

And I can modify this dimension value,

08:39

say down to 12 or up to 14 and have

08:43

that line adjust its position figuring out these references.

08:47

It's going to be an important aspect of building a parametric design,

08:50

understanding how you want to dimension something so that it can update properly.

08:55

Next we're going to finish the sketch and we'll

08:56

be using this to create the solid body.

08:59

Well, first begin by extruding the smaller section,

09:02

I'm going to use the direction set to symmetric,

09:06

set the measurement value so that it's the full length

09:09

And this section is going to be a distance of 7.45 mm.

09:14

We'll need to expand the sketches and bring the sketch back.

09:17

We're going to exclude the other side,

09:19

making sure to include everything with the exception of these small sections.

09:23

Once again using symmetric setting it to the full length and

09:28

this side is going to be a distance of 13 mm.

09:32

We're going to right click and repeat the extrude

09:34

this time. We're going to extrude the center section.

09:37

This is going to be symmetric again the whole length and 6.5 mm.

09:43

Now we need to remove the section from the center.

09:46

Once again we can right click and repeat the

09:48

extrude and we can select the center section.

09:52

We need to hold down control or command to select multiple profiles.

09:56

Use the symmetric option the whole length one more

09:59

time and the distance between these is 4.65 mm.

10:04

Now that we've removed all of that information.

10:06

We can hide the sketch, we can hide our crank arm and we can apply some filets.

10:11

So from modify fill it.

10:13

I'm going to select the two vertical edges on the big

10:16

side and the two vertical edges on the smaller side.

10:19

And I'm going to apply a five millimeter Philip.

10:22

I'm going to right click and repeat this and apply it to the top and bottom.

10:26

This time I'm going to use the on screen manipulator and drag this out

10:30

and in this case 5.5 millimeters. And hit enter too. Okay,

10:35

so now we've recreated the link using a single sketch and

10:39

all the dimensions required as well as a handful of features.

10:42

Now we have a fully featured parametric version of this link.

10:46

We don't have the recesses or the text that was included on the original.

10:50

But all the critical features, including the hole diameters,

10:53

thicknesses and required geometry are there at this point.

10:57

Let's make sure that we do save our new link.

10:59

And instead of doing a save, I'm going to do a save as

11:03

notice that I have another folder in this case,

11:06

I want to go back and go into my parametric

11:08

modeling folder and I'm going to call this one parametric link

11:13

from here.

11:13

Continue to make any adjustments or modifications that you see fit

11:16

and then make sure that you save it before moving on.

Video quiz

Which of the following Create tools becomes available after Capture Design History is disabled?

(Select one)
Select an answer

1/1 questions left unanswered

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