How to add dimensions and constraints

00:02

How to add dimensions and constraints.

00:06

After completing this video,

00:07

you'll be able to create a sketch dimension,

00:09

create a sketch constraint,

00:11

link sketch dimensions,

00:13

and create and link user parameters.

00:17

To get started in Fusion,

00:18

we want to begin with a new untitled document.

00:21

We're gonna start first by creating a new sketch on the front plane.

00:25

When we start our new sketch,

00:26

we're going to begin with the line tool.

00:28

We're gonna start by dragging the line tool vertically.

00:31

By default,

00:32

we'll have dimension input boxes on the screen.

00:36

If we click to place the line,

00:37

those dimension boxes will disappear.

00:40

As we continue to create lines,

00:42

there are some instances where we're going to

00:44

get default constraints or persistent constraints added.

00:48

As we get a line closer to horizontal,

00:51

you can see that it's trying to apply a perpendicular constraint.

00:54

As we get it closer to vertical,

00:56

it may have a perpendicular constraint,

00:58

a parallel constraint,

00:59

or a coincident constraint with other geometry.

01:02

If we go back to the origin.

01:05

You can see that it's closing off the profile,

01:07

and there are some sketch constraint icons that are listed.

01:11

Let's hit escape to get off our line tool and let's identify them.

01:14

This constraint here is a vertical constraint,

01:17

meaning this line is vertical in relation to our coordinate system.

01:21

This constraint icon here is perpendicular,

01:24

meaning these two lines are 90 degrees to each other.

01:27

Same thing with this one here.

01:29

Any time we click on a constraint,

01:30

it'll highlight the geometry.

01:32

In some cases,

01:34

such as clicking at the origin,

01:35

you'll notice that a coincident constraint appears.

01:38

The coincidence constraints oftentimes are hidden until you select the geometry.

01:43

This means that we've got two lines that are coincident with each other,

01:47

as well as a line coincident with the origin.

01:50

This sketch here is still underdefined,

01:52

meaning that we can move it about because we haven't

01:55

added any dimensions or fully defined it with constraints.

01:58

We can use constraints to lock down the majority

02:01

of our sketches by using constraints such as equal,

02:05

for example,

02:05

making this vertical and horizontal line equal.

02:09

We can also add perpendicular,

02:11

horizontal,

02:12

vertical,

02:12

parallel,

02:13

or co-linear constraints.

02:15

For example,

02:16

if we always want this line to be horizontal,

02:19

we simply need to click on it.

02:21

For the constraint horizontal vertical,

02:23

it'll be applied to the closest variation of that.

02:26

For example,

02:27

if we have a line

02:28

that is near vertical,

02:31

or if we have a line that's near horizontal.

02:34

The line that's near vertical will end up with the vertical constraint.

02:37

The one that's near horizontal will end up with a horizontal constraint.

02:41

When you're manually creating sketch entities,

02:44

there's generally no case where it'll be exactly 45 degrees.

02:48

So it'll either go to a vertical or a

02:50

horizontal variation based on where its current position is.

02:55

This sketch rectangle here is not fully defined yet,

02:58

but you'll notice that because of our equal constraint,

03:00

it is now defined as a perfect square.

03:03

To fully define this,

03:04

we'll have to add what's called a dimension.

03:07

Now dimensions can be added at the time of creation,

03:09

but we can also apply them after the fact.

03:12

Let's go ahead and add a horizontal dimension of 50 millimeters.

03:16

We can see here now that the sketch is fully defined.

03:19

All the sketch entities are black,

03:20

and if we expand our sketches folder,

03:22

we can see the lock icon.

03:24

Let's go ahead and hit escape.

03:27

I'm gonna add a few more sketch entities.

03:30

In this case,

03:31

let's just add 3 circles

03:32

and hit escape.

03:34

When we apply a dimension to a circle,

03:37

it's going to automatically be a diameter if it's a complete circle,

03:40

or it'll be a radius value if it's an open arc.

03:43

We also have the ability to right click and

03:45

change the type of dimension that we're adding.

03:48

For example,

03:48

if we want to drive this as a radius value,

03:51

or we can right click and drive it as a diameter value.

03:54

Let's enter 35 for this one.

03:57

Sketch dimensions can also be reference dimensions.

04:01

For example,

04:01

we have an equal constraint that makes this a true square.

04:05

However,

04:05

we only added a dimension to the horizontal line.

04:08

If we wanted to validate this,

04:10

we could add a dimension to the vertical line,

04:12

and this would automatically be created as a driven dimension.

04:16

This means that it's going to have brackets around it,

04:18

and this dimension specifically is a reference value.

04:22

If we hit escape to get off our dimension tool and double click to modify this to 75,

04:27

notice that they both update.

04:29

Reference dimensions can be helpful because we can gather information about

04:33

a design that maybe is outside of the design intent.

04:36

For example,

04:37

understanding the distance between these two points.

04:40

We can see here that this driven dimension is 106.066 millimeters.

04:47

We also can convert dimensions to driven dimensions,

04:50

so if we hit a skate.

04:52

And select a dimension,

04:54

right click,

04:55

we can toggle this as driven.

04:57

As soon as we toggle it as driven,

04:58

the sketch is no longer fully defined.

05:01

However,

05:02

we have the ability to also toggle this one,

05:04

so we'll select the dimension,

05:06

right click,

05:06

and toggle it as driving.

05:08

If we need the aligned distance to always be 100 millimeters,

05:11

we can drive it from point to point,

05:14

and then we can get a dimension as a reference for the overall width and length.

05:19

There are many different ways that we can use dimensions and sketches,

05:22

and it's always a good idea to practice and play around with each sketch entity

05:26

and how you can fully define it.

05:29

In most cases,

05:30

you may find that you use more constraints and dimensions whenever possible.

05:34

For example,

05:35

if we want these holes to be horizontal

05:38

and we want it to be horizontal relative to

05:40

this point or vertical relative to this point,

05:43

we can make those adjustments or changes simply by adding the constraints.

05:47

We can also ensure that they're tangent relative to each other

05:51

and that it's tangent relative to a reference line.

05:54

You'll notice that if we try to overdefine a constraint,

05:57

for example,

05:58

we've got a vertical constraint with this point and we try to apply a tangency,

06:02

that fusion will not allow it.

06:04

We have to remove one of the constraints in order to validate that.

06:07

So we'll hit escape.

06:09

We'll find the center point location

06:11

and we'll delete by selecting and hitting delete on the keyboard

06:15

that constraint that was overdefining it.

06:18

Next,

06:18

we can use equal to make sure all three of these circles are the same size,

06:22

and now we can apply our tangency constraint here.

06:26

To fully define this,

06:27

we can also add something like a dimension.

06:30

In this case,

06:30

it can be a vertical dimension,

06:33

a horizontal dimension,

06:35

or what's called an aligned dimension.

06:37

If you have trouble figuring out which one to use,

06:39

you can always right click and you can lock it in a specific orientation.

06:44

For example,

06:44

if I always want this to be aligned,

06:46

I can pull it down and say this always needs to be 20 millimeters.

06:50

It'll drive the position of all three of those circles

06:53

based on this one dimension.

06:56

Now that we have some of the basics down,

06:57

let's go ahead and hide the sketch and let's create a new one.

07:02

Now let's take a look at a common example.

07:05

We're going to begin by creating a center point rectangle.

07:08

And we're going to define the dimensions while they're being created,

07:14

Next,

07:15

we're going to add a sketch circle.

07:18

We're gonna add a dimension.

07:21

Making this 15 millimeter diameter.

07:24

And then we're going to add a distance from this vertical edge.

07:27

I'm gonna say that I always want this to be 10 millimeters away from that edge.

07:32

In order for me to have a consistent scheme or a consistent way to define my sketch,

07:38

it's a good idea to consider linking dimensions together.

07:42

In some cases,

07:43

it's easier for us to use dimensions that

07:45

are linked together rather than using constraints.

07:48

In a situation like this,

07:49

we may want to define the horizontal distance between this hole

07:53

by selecting the distance we applied to the vertical

07:57

and hitting enter.

07:58

This means that these two values are now linked together.

08:01

If I modify one,

08:03

the other one is going to change.

08:06

This is a convenient way to fully define your sketches without the

08:09

need to create additional construction geometry and using the equal constraint.

08:14

In some instances you may find that you want to predefine some of these values.

08:18

In those cases,

08:19

you can use the modify change parameters option,

08:23

and we can select the plus icon.

08:25

In this case,

08:26

I'm going to create a value called DIA for diameter.

08:30

The expression for this is gonna be 15 millimeters and I'll hit enter.

08:35

If I want to link this value when I'm creating my dimension,

08:38

all I need to do is start to type in D for diameter.

08:42

A dialogue will pop up and I hit enter,

08:44

and this will now link this to my diameter parameter.

08:48

If I go to modify and change parameters,

08:51

let's go ahead and minimize this.

08:53

And bring it down.

08:55

We can modify the expression.

08:57

Instead of 15 millimeters,

08:59

let's say this needs to be 12.

09:01

It'll update my sketch because the values are linked together.

09:04

We can also use parameters as well as

09:06

general input values to use mathematical operators.

09:11

For example,

09:12

instead of 10 millimeters here,

09:13

let's say that I wanted it to be the diameter

09:16

plus 2 millimeters.

09:18

This means that this diameter value is not only controlling the size of our circle,

09:23

but it also has an effect on its position.

09:26

If I were to go back into my modified change parameters

09:29

and change this to say 10 millimeters.

09:32

The whole size and its location is gonna update.

09:36

Playing around with the way in which sketches are defined takes a good bit of time.

09:40

Understanding the design implications and the downstream effects of the way a

09:44

sketch is defined is something that will come with lots of practice.

09:48

But make sure that you understand the

09:50

basics of creating sketch dimensions and constraints,

09:53

linking sketch dimensions together,

09:55

as well as creating basic user parameters

09:57

for things like diameters and distance values.

10:00

And once you have that,

10:01

you'll be able to link those to your

10:02

sketches and create a more robust parametric model.

10:06

We're not gonna be using this design,

10:08

but if you feel like you want to continue to play with it,

10:10

make sure that you do save it before moving on.

Video transcript

00:02

How to add dimensions and constraints.

00:06

After completing this video,

00:07

you'll be able to create a sketch dimension,

00:09

create a sketch constraint,

00:11

link sketch dimensions,

00:13

and create and link user parameters.

00:17

To get started in Fusion,

00:18

we want to begin with a new untitled document.

00:21

We're gonna start first by creating a new sketch on the front plane.

00:25

When we start our new sketch,

00:26

we're going to begin with the line tool.

00:28

We're gonna start by dragging the line tool vertically.

00:31

By default,

00:32

we'll have dimension input boxes on the screen.

00:36

If we click to place the line,

00:37

those dimension boxes will disappear.

00:40

As we continue to create lines,

00:42

there are some instances where we're going to

00:44

get default constraints or persistent constraints added.

00:48

As we get a line closer to horizontal,

00:51

you can see that it's trying to apply a perpendicular constraint.

00:54

As we get it closer to vertical,

00:56

it may have a perpendicular constraint,

00:58

a parallel constraint,

00:59

or a coincident constraint with other geometry.

01:02

If we go back to the origin.

01:05

You can see that it's closing off the profile,

01:07

and there are some sketch constraint icons that are listed.

01:11

Let's hit escape to get off our line tool and let's identify them.

01:14

This constraint here is a vertical constraint,

01:17

meaning this line is vertical in relation to our coordinate system.

01:21

This constraint icon here is perpendicular,

01:24

meaning these two lines are 90 degrees to each other.

01:27

Same thing with this one here.

01:29

Any time we click on a constraint,

01:30

it'll highlight the geometry.

01:32

In some cases,

01:34

such as clicking at the origin,

01:35

you'll notice that a coincident constraint appears.

01:38

The coincidence constraints oftentimes are hidden until you select the geometry.

01:43

This means that we've got two lines that are coincident with each other,

01:47

as well as a line coincident with the origin.

01:50

This sketch here is still underdefined,

01:52

meaning that we can move it about because we haven't

01:55

added any dimensions or fully defined it with constraints.

01:58

We can use constraints to lock down the majority

02:01

of our sketches by using constraints such as equal,

02:05

for example,

02:05

making this vertical and horizontal line equal.

02:09

We can also add perpendicular,

02:11

horizontal,

02:12

vertical,

02:12

parallel,

02:13

or co-linear constraints.

02:15

For example,

02:16

if we always want this line to be horizontal,

02:19

we simply need to click on it.

02:21

For the constraint horizontal vertical,

02:23

it'll be applied to the closest variation of that.

02:26

For example,

02:27

if we have a line

02:28

that is near vertical,

02:31

or if we have a line that's near horizontal.

02:34

The line that's near vertical will end up with the vertical constraint.

02:37

The one that's near horizontal will end up with a horizontal constraint.

02:41

When you're manually creating sketch entities,

02:44

there's generally no case where it'll be exactly 45 degrees.

02:48

So it'll either go to a vertical or a

02:50

horizontal variation based on where its current position is.

02:55

This sketch rectangle here is not fully defined yet,

02:58

but you'll notice that because of our equal constraint,

03:00

it is now defined as a perfect square.

03:03

To fully define this,

03:04

we'll have to add what's called a dimension.

03:07

Now dimensions can be added at the time of creation,

03:09

but we can also apply them after the fact.

03:12

Let's go ahead and add a horizontal dimension of 50 millimeters.

03:16

We can see here now that the sketch is fully defined.

03:19

All the sketch entities are black,

03:20

and if we expand our sketches folder,

03:22

we can see the lock icon.

03:24

Let's go ahead and hit escape.

03:27

I'm gonna add a few more sketch entities.

03:30

In this case,

03:31

let's just add 3 circles

03:32

and hit escape.

03:34

When we apply a dimension to a circle,

03:37

it's going to automatically be a diameter if it's a complete circle,

03:40

or it'll be a radius value if it's an open arc.

03:43

We also have the ability to right click and

03:45

change the type of dimension that we're adding.

03:48

For example,

03:48

if we want to drive this as a radius value,

03:51

or we can right click and drive it as a diameter value.

03:54

Let's enter 35 for this one.

03:57

Sketch dimensions can also be reference dimensions.

04:01

For example,

04:01

we have an equal constraint that makes this a true square.

04:05

However,

04:05

we only added a dimension to the horizontal line.

04:08

If we wanted to validate this,

04:10

we could add a dimension to the vertical line,

04:12

and this would automatically be created as a driven dimension.

04:16

This means that it's going to have brackets around it,

04:18

and this dimension specifically is a reference value.

04:22

If we hit escape to get off our dimension tool and double click to modify this to 75,

04:27

notice that they both update.

04:29

Reference dimensions can be helpful because we can gather information about

04:33

a design that maybe is outside of the design intent.

04:36

For example,

04:37

understanding the distance between these two points.

04:40

We can see here that this driven dimension is 106.066 millimeters.

04:47

We also can convert dimensions to driven dimensions,

04:50

so if we hit a skate.

04:52

And select a dimension,

04:54

right click,

04:55

we can toggle this as driven.

04:57

As soon as we toggle it as driven,

04:58

the sketch is no longer fully defined.

05:01

However,

05:02

we have the ability to also toggle this one,

05:04

so we'll select the dimension,

05:06

right click,

05:06

and toggle it as driving.

05:08

If we need the aligned distance to always be 100 millimeters,

05:11

we can drive it from point to point,

05:14

and then we can get a dimension as a reference for the overall width and length.

05:19

There are many different ways that we can use dimensions and sketches,

05:22

and it's always a good idea to practice and play around with each sketch entity

05:26

and how you can fully define it.

05:29

In most cases,

05:30

you may find that you use more constraints and dimensions whenever possible.

05:34

For example,

05:35

if we want these holes to be horizontal

05:38

and we want it to be horizontal relative to

05:40

this point or vertical relative to this point,

05:43

we can make those adjustments or changes simply by adding the constraints.

05:47

We can also ensure that they're tangent relative to each other

05:51

and that it's tangent relative to a reference line.

05:54

You'll notice that if we try to overdefine a constraint,

05:57

for example,

05:58

we've got a vertical constraint with this point and we try to apply a tangency,

06:02

that fusion will not allow it.

06:04

We have to remove one of the constraints in order to validate that.

06:07

So we'll hit escape.

06:09

We'll find the center point location

06:11

and we'll delete by selecting and hitting delete on the keyboard

06:15

that constraint that was overdefining it.

06:18

Next,

06:18

we can use equal to make sure all three of these circles are the same size,

06:22

and now we can apply our tangency constraint here.

06:26

To fully define this,

06:27

we can also add something like a dimension.

06:30

In this case,

06:30

it can be a vertical dimension,

06:33

a horizontal dimension,

06:35

or what's called an aligned dimension.

06:37

If you have trouble figuring out which one to use,

06:39

you can always right click and you can lock it in a specific orientation.

06:44

For example,

06:44

if I always want this to be aligned,

06:46

I can pull it down and say this always needs to be 20 millimeters.

06:50

It'll drive the position of all three of those circles

06:53

based on this one dimension.

06:56

Now that we have some of the basics down,

06:57

let's go ahead and hide the sketch and let's create a new one.

07:02

Now let's take a look at a common example.

07:05

We're going to begin by creating a center point rectangle.

07:08

And we're going to define the dimensions while they're being created,

07:14

Next,

07:15

we're going to add a sketch circle.

07:18

We're gonna add a dimension.

07:21

Making this 15 millimeter diameter.

07:24

And then we're going to add a distance from this vertical edge.

07:27

I'm gonna say that I always want this to be 10 millimeters away from that edge.

07:32

In order for me to have a consistent scheme or a consistent way to define my sketch,

07:38

it's a good idea to consider linking dimensions together.

07:42

In some cases,

07:43

it's easier for us to use dimensions that

07:45

are linked together rather than using constraints.

07:48

In a situation like this,

07:49

we may want to define the horizontal distance between this hole

07:53

by selecting the distance we applied to the vertical

07:57

and hitting enter.

07:58

This means that these two values are now linked together.

08:01

If I modify one,

08:03

the other one is going to change.

08:06

This is a convenient way to fully define your sketches without the

08:09

need to create additional construction geometry and using the equal constraint.

08:14

In some instances you may find that you want to predefine some of these values.

08:18

In those cases,

08:19

you can use the modify change parameters option,

08:23

and we can select the plus icon.

08:25

In this case,

08:26

I'm going to create a value called DIA for diameter.

08:30

The expression for this is gonna be 15 millimeters and I'll hit enter.

08:35

If I want to link this value when I'm creating my dimension,

08:38

all I need to do is start to type in D for diameter.

08:42

A dialogue will pop up and I hit enter,

08:44

and this will now link this to my diameter parameter.

08:48

If I go to modify and change parameters,

08:51

let's go ahead and minimize this.

08:53

And bring it down.

08:55

We can modify the expression.

08:57

Instead of 15 millimeters,

08:59

let's say this needs to be 12.

09:01

It'll update my sketch because the values are linked together.

09:04

We can also use parameters as well as

09:06

general input values to use mathematical operators.

09:11

For example,

09:12

instead of 10 millimeters here,

09:13

let's say that I wanted it to be the diameter

09:16

plus 2 millimeters.

09:18

This means that this diameter value is not only controlling the size of our circle,

09:23

but it also has an effect on its position.

09:26

If I were to go back into my modified change parameters

09:29

and change this to say 10 millimeters.

09:32

The whole size and its location is gonna update.

09:36

Playing around with the way in which sketches are defined takes a good bit of time.

09:40

Understanding the design implications and the downstream effects of the way a

09:44

sketch is defined is something that will come with lots of practice.

09:48

But make sure that you understand the

09:50

basics of creating sketch dimensions and constraints,

09:53

linking sketch dimensions together,

09:55

as well as creating basic user parameters

09:57

for things like diameters and distance values.

10:00

And once you have that,

10:01

you'll be able to link those to your

10:02

sketches and create a more robust parametric model.

10:06

We're not gonna be using this design,

10:08

but if you feel like you want to continue to play with it,

10:10

make sure that you do save it before moving on.

After completing this video, you'll be able to:

  • Create a sketch dimension.
  • Create a sketch constraint.
  • Link sketch dimensions.
  • Create and link a user parameters.

Video quiz

How is a driven dimension of 75.00 displayed in a sketch?

(Select one)
Select an answer

1/1 questions left unanswered

Step-by-step guide

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