& Construction
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Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
& Manufacturing
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Professional CAD/CAM tools built on Inventor and AutoCAD
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.
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:
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