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After completing this video, you will be able to:
Transcript
00:02
Create and modify sketches.
00:05
After completing this video, you'll be able to create a sketch,
00:09
apply dimensions to a sketch, apply constraints to a sketch,
00:12
select and delete a sketch constraint
00:15
and create a sketch projection from an edge or face
00:21
to get started in fusion. We want to open the supplied data set locking ring dot F 3D.
00:26
This design contains a single solid body as well as four different sketches.
00:31
We can see all the sketches that went in to create this original part.
00:35
In this video.
00:36
We're going to be talking about the creation and modification
00:39
of sketches as they are the foundation to parametric modeling
00:43
to get started. We first need to understand how to create a sketch
00:46
to create a sketch. We either need a plane
00:49
or a planar face.
00:51
When we select the create sketch button,
00:53
notice the default origin planes will show up on the screen.
00:57
If we simply hover around into different orientations,
00:59
we can see that the grid changes to the different planes.
01:03
We can also select the planes by holding down the left mouse button.
01:06
If we're selecting through solid geometry and pick the plane that we want to use
01:11
sketch plans should be used for the basis of all your sketches.
01:14
But in some instances, you may find that you want to use a planar face instead.
01:19
In this case, let's go ahead and select the top of the solid body.
01:23
When we create a sketch on the selected face,
01:26
we're automatically going to get sketch profiles
01:29
that come into our current sketch.
01:31
If I hide the body
01:32
and I select the profile on the screen,
01:35
we can see that we've brought that geometry into our current sketch.
01:39
So creating a sketch on a planar face is going to allow us
01:42
to access and use that geometry without projecting it into the current sketch.
01:47
This means that if we want to replicate geometry or use it as a reference,
01:51
this makes the process relatively easy.
01:54
Let's talk a bit about creating sketches themselves.
01:58
There are many different creation tools that we can have access to
02:01
lions, different types of rectangles, circles and arcs,
02:04
polygons and some more advanced tools, things like ellipses,
02:08
blinds and conic curves.
02:10
Let's focus on some of the basic tools.
02:13
If we wanted to create a line,
02:14
we simply need to left click at the start point of our line.
02:17
In this case, let's left click at the origin
02:19
and then begin dragging out and snapping to the next location.
02:24
By default fusion will have what are called persistent constraints,
02:28
which means that if you're close to vertical,
02:30
it's gonna apply a vertical constraint.
02:32
If you're close to horizontal, it will apply a horizontal constraint.
02:36
If you're near other geometry, say a midpoint, you may see a triangle icon
02:41
and it'll snap to that geometry.
02:43
These persistent constraints can be overridden by holding down the control key
02:47
on a windows machine or the command key on the mac.
02:50
If we're going to snap to a location, we simply need to left click to end the line tool.
02:55
When we're using the line tool, we also have the ability to go back to the last point.
02:60
Hold down the left mouse button and convert this to a tangent arc.
03:04
This can be extremely helpful as we're creating more complex sketches
03:08
to finish a line.
03:09
We can either hit the green check mark which will keep the line tool active
03:13
or we can hit escape which will end the line tool altogether.
03:16
Let's go ahead and select these lines and delete them as they aren't needed.
03:21
Next, we wanna talk about creating a construction line.
03:25
Any geometry in a sketch can be converted to a construction line.
03:29
If we select this line in our sketch palette, we can select construction
03:34
and this will turn this into a construction line.
03:36
Construction lines are used as references and are not part of any sketch profiles.
03:42
So in this case, this line can be here and used as a reference.
03:45
However,
03:46
it doesn't have any impact on any closed profiles
03:48
that we select to use for things like extrude.
03:51
Let's go ahead and add one more line. In
03:53
this case, we're gonna select that center point drag down to about 0.75 inches
03:59
and then we'll hit escape to get off the line tool.
04:02
This line is currently under defined.
04:04
It has an automatic parallel constraint that's been added,
04:08
making it parallel to this original line,
04:10
but the end point is white and it allows us to drag it and change the overall length.
04:16
In some cases,
04:17
you may find that you want to apply a dimension to fully define your sketch.
04:21
While in other cases, constraints make more sense.
04:24
This is a case by case basis.
04:26
But in general, we have to think about how we expect the sketch to update downstream.
04:32
In this case, if I wanted to replicate this feature on the other side,
04:35
but didn't want to use a pattern or a mirror feature,
04:39
I could use the equal constraint to ensure that this
04:42
line and this line are always the same length.
04:45
Then I can use my circle tool
04:48
and I can start a circle snapping to this point.
04:51
And I can use additional constraints such as coincident
04:55
to ensure that it snaps to this end position.
04:58
Then we can use other constraints such as horizontal vertical
05:02
to ensure that it's either horizontal or vertical with another selected point.
05:07
By default fusion will go to the closest version.
05:10
In this case, horizontal was closer than vertical.
05:13
So you may find that you need to undo that last selection
05:17
and drag it into a position that's closer to vertical.
05:21
Now, we can use horizontal, vertical and make that position known.
05:25
Now, we've been able to replicate the geometry from this upper section
05:29
by using only constraints and no dimensions.
05:33
While constraints are great,
05:34
they won't get you a fully defined sketch in every case.
05:37
So let's explore creating our own fully defined sketches.
05:41
I'm gonna start by using the rectangle tool.
05:43
And in my sketch palette, I wanna change this to a center rectangle.
05:47
This will add some additional construction geometry allowing
05:50
us to create a rectangle from the origin.
05:53
By default,
05:54
we'll be able to enter dimensions on the fly while creating our sketch rectangle.
05:58
You can see that the horizontal dimension is currently highlighted
06:02
if I enter one inch and then I hit tab to go to the next box,
06:06
I can enter 0.75 inches and you can see there's a lock icon next to both of those.
06:11
If I hit the enter key, I will accept that.
06:14
And now I've created a one by 0.75 inch rectangle in the center of my part.
06:19
Next, let's go ahead and use the center diameter circle
06:23
as we're dragging the center diameter circle out. Let's not apply a dimension.
06:27
Let's simply left click and then it escaped to get off of the sketch tool.
06:31
In this instance, there are a few ways that we could define the circle.
06:35
For example,
06:36
we could use a coincident constraint between the
06:38
circle and one of these corner points.
06:40
This will allow us to fully define that sketch.
06:43
Let's undo this.
06:45
You can use control Z on the keyboard or you can use the undo option at the top.
06:49
And let's apply a dimension.
06:52
In this case, the dimension I want is going to be
06:56
one inch
06:57
and then I'm going to use some mathematical operators here plus a quarter inch
07:02
and we'll hit enter
07:03
what this allows us to do is drive the
07:05
diameter of the circle relative to other dimensions.
07:08
In the sketch.
07:09
For example, if I were to change this one inch value to 1.25 or two inches,
07:15
then you can see the overall sketches updated,
07:18
the rectangle updated as well as this large circle.
07:21
If I take this back down to one inch, you can see that everything changes as well.
07:26
So it's important to think about how your sketches are going to update.
07:30
If you always want this circle to be coincident
07:33
or intersect with the corner point of a rectangle,
07:35
then using a constraint is the best way.
07:38
However,
07:38
if you want the circle's diameter to be relative
07:41
to some other value or dimension in your sketch,
07:44
then making some sort of mathematical operator or equation allowing
07:48
you to drive that makes a little bit more sense
07:51
at any point in time we can change or
07:53
delete the constraints and dimensions in our sketch.
07:56
For example, I can select this and hit delete on the keyboard to get rid of it.
08:01
Then I can decide that I want to use that coincident constraint. After all,
08:05
if we have a coincident constraint or some other constraint,
08:08
and we decide that we don't want to use that,
08:10
we can always go back and change that as well.
08:12
Let's hit escape to get off our constraint tool and let's find
08:16
and select the parallel constraint that was added to our vertical line
08:20
with it selected,
08:21
it'll highlight the other constraint as well as the sketch geometry.
08:24
We simply need to hit delete on the keyboard
08:27
and now we can move this geometry around.
08:30
However, in this instance,
08:31
you'll note now the vertical constraint is likely
08:34
not the right constraint for the job.
08:36
So we're gonna select and delete the vertical constraint.
08:40
Now we want to use coincident between this line and this center point.
08:45
And while there's not a situation where those can touch
08:48
using the coincident constraint in this instance,
08:50
will allow us to take the extension of this line and make
08:53
sure that it always intersects the center point of that circle.
08:56
We can hit escape on the keyboard
08:58
and now we can drag this around to other positions.
09:01
So this is a great instance where using a constraint as well
09:04
as some dimensions to dictate a new position makes the most sense
09:09
if I needed that new feature to be at 60 degrees.
09:12
Now, I have a way that I can control it with both dimensions as well as constraints.
09:17
In some cases, you'll have all the information you need inside of a single sketch.
09:22
But in other instances, you may find that you need to go to your project,
09:25
include tools and project geometry from some other reference in your design.
09:30
In most cases, the project tool is used to gather information about your design.
09:34
For example, the inside diameter of this lower edge,
09:38
we're gonna say OK, and go back to our top view.
09:42
Notice that the projected geometry comes in as purple.
09:45
I'm gonna temporarily hide the body to make this a little bit easier to see.
09:49
This is a great way for us to bring in additional references.
09:53
And if they're not needed for sketch profiles,
09:55
we can select them and convert them to construction.
09:58
This means that they won't participate in the selection of those features.
10:02
For example, if this inside section isn't needed for our extrude,
10:07
we can select this curve
10:09
and make it construction.
10:11
This means that our only valid profile selections are now going to be inside of
10:14
this circle as well as the circle and rectangle in the center of our design.
10:20
We can also double click on sketch entities to get an entire profile.
10:24
And in this case, convert that to construction,
10:27
this allows us to have the geometry we need easily as well
10:30
as all the reference geometry to help drive the overall dimensions.
10:34
Understanding how a sketch is going to influence your design downstream,
10:38
takes a lot of practice and trial and error.
10:40
Once you have enough time using fusion and creating your own sketches,
10:45
you'll begin to understand how these initial decisions
10:47
on creating sketches will have a downstream effect.
10:51
But the good news is you can always go back to
10:53
these sketches at any point in time and make adjustments.
10:56
For example, I can double click on the original sketch used to drive this design
10:60
and I can make a change here.
11:02
If I make a change here, it's going to affect the overall design,
11:06
including the solid body and any additional geometry.
11:10
We can see that the position of this circle has updated
11:13
and we can make those changes once more by right clicking and showing the dimensions
11:20
and then making the change on the screen. So we can see the updates happen
11:24
playing around with simple designs is a great way to better understand the
11:27
limits and the constraints placed on your designs by these initial sketches.
11:31
So make sure that you spend enough time
11:33
getting comfortable with creating some basic sketch elements,
11:36
make sure that you apply dimensions and constraints
11:39
and come up with some examples of your own to figure out how to best use these.
11:43
Once you're done, let's go ahead and move on to the next step.
Video transcript
00:02
Create and modify sketches.
00:05
After completing this video, you'll be able to create a sketch,
00:09
apply dimensions to a sketch, apply constraints to a sketch,
00:12
select and delete a sketch constraint
00:15
and create a sketch projection from an edge or face
00:21
to get started in fusion. We want to open the supplied data set locking ring dot F 3D.
00:26
This design contains a single solid body as well as four different sketches.
00:31
We can see all the sketches that went in to create this original part.
00:35
In this video.
00:36
We're going to be talking about the creation and modification
00:39
of sketches as they are the foundation to parametric modeling
00:43
to get started. We first need to understand how to create a sketch
00:46
to create a sketch. We either need a plane
00:49
or a planar face.
00:51
When we select the create sketch button,
00:53
notice the default origin planes will show up on the screen.
00:57
If we simply hover around into different orientations,
00:59
we can see that the grid changes to the different planes.
01:03
We can also select the planes by holding down the left mouse button.
01:06
If we're selecting through solid geometry and pick the plane that we want to use
01:11
sketch plans should be used for the basis of all your sketches.
01:14
But in some instances, you may find that you want to use a planar face instead.
01:19
In this case, let's go ahead and select the top of the solid body.
01:23
When we create a sketch on the selected face,
01:26
we're automatically going to get sketch profiles
01:29
that come into our current sketch.
01:31
If I hide the body
01:32
and I select the profile on the screen,
01:35
we can see that we've brought that geometry into our current sketch.
01:39
So creating a sketch on a planar face is going to allow us
01:42
to access and use that geometry without projecting it into the current sketch.
01:47
This means that if we want to replicate geometry or use it as a reference,
01:51
this makes the process relatively easy.
01:54
Let's talk a bit about creating sketches themselves.
01:58
There are many different creation tools that we can have access to
02:01
lions, different types of rectangles, circles and arcs,
02:04
polygons and some more advanced tools, things like ellipses,
02:08
blinds and conic curves.
02:10
Let's focus on some of the basic tools.
02:13
If we wanted to create a line,
02:14
we simply need to left click at the start point of our line.
02:17
In this case, let's left click at the origin
02:19
and then begin dragging out and snapping to the next location.
02:24
By default fusion will have what are called persistent constraints,
02:28
which means that if you're close to vertical,
02:30
it's gonna apply a vertical constraint.
02:32
If you're close to horizontal, it will apply a horizontal constraint.
02:36
If you're near other geometry, say a midpoint, you may see a triangle icon
02:41
and it'll snap to that geometry.
02:43
These persistent constraints can be overridden by holding down the control key
02:47
on a windows machine or the command key on the mac.
02:50
If we're going to snap to a location, we simply need to left click to end the line tool.
02:55
When we're using the line tool, we also have the ability to go back to the last point.
02:60
Hold down the left mouse button and convert this to a tangent arc.
03:04
This can be extremely helpful as we're creating more complex sketches
03:08
to finish a line.
03:09
We can either hit the green check mark which will keep the line tool active
03:13
or we can hit escape which will end the line tool altogether.
03:16
Let's go ahead and select these lines and delete them as they aren't needed.
03:21
Next, we wanna talk about creating a construction line.
03:25
Any geometry in a sketch can be converted to a construction line.
03:29
If we select this line in our sketch palette, we can select construction
03:34
and this will turn this into a construction line.
03:36
Construction lines are used as references and are not part of any sketch profiles.
03:42
So in this case, this line can be here and used as a reference.
03:45
However,
03:46
it doesn't have any impact on any closed profiles
03:48
that we select to use for things like extrude.
03:51
Let's go ahead and add one more line. In
03:53
this case, we're gonna select that center point drag down to about 0.75 inches
03:59
and then we'll hit escape to get off the line tool.
04:02
This line is currently under defined.
04:04
It has an automatic parallel constraint that's been added,
04:08
making it parallel to this original line,
04:10
but the end point is white and it allows us to drag it and change the overall length.
04:16
In some cases,
04:17
you may find that you want to apply a dimension to fully define your sketch.
04:21
While in other cases, constraints make more sense.
04:24
This is a case by case basis.
04:26
But in general, we have to think about how we expect the sketch to update downstream.
04:32
In this case, if I wanted to replicate this feature on the other side,
04:35
but didn't want to use a pattern or a mirror feature,
04:39
I could use the equal constraint to ensure that this
04:42
line and this line are always the same length.
04:45
Then I can use my circle tool
04:48
and I can start a circle snapping to this point.
04:51
And I can use additional constraints such as coincident
04:55
to ensure that it snaps to this end position.
04:58
Then we can use other constraints such as horizontal vertical
05:02
to ensure that it's either horizontal or vertical with another selected point.
05:07
By default fusion will go to the closest version.
05:10
In this case, horizontal was closer than vertical.
05:13
So you may find that you need to undo that last selection
05:17
and drag it into a position that's closer to vertical.
05:21
Now, we can use horizontal, vertical and make that position known.
05:25
Now, we've been able to replicate the geometry from this upper section
05:29
by using only constraints and no dimensions.
05:33
While constraints are great,
05:34
they won't get you a fully defined sketch in every case.
05:37
So let's explore creating our own fully defined sketches.
05:41
I'm gonna start by using the rectangle tool.
05:43
And in my sketch palette, I wanna change this to a center rectangle.
05:47
This will add some additional construction geometry allowing
05:50
us to create a rectangle from the origin.
05:53
By default,
05:54
we'll be able to enter dimensions on the fly while creating our sketch rectangle.
05:58
You can see that the horizontal dimension is currently highlighted
06:02
if I enter one inch and then I hit tab to go to the next box,
06:06
I can enter 0.75 inches and you can see there's a lock icon next to both of those.
06:11
If I hit the enter key, I will accept that.
06:14
And now I've created a one by 0.75 inch rectangle in the center of my part.
06:19
Next, let's go ahead and use the center diameter circle
06:23
as we're dragging the center diameter circle out. Let's not apply a dimension.
06:27
Let's simply left click and then it escaped to get off of the sketch tool.
06:31
In this instance, there are a few ways that we could define the circle.
06:35
For example,
06:36
we could use a coincident constraint between the
06:38
circle and one of these corner points.
06:40
This will allow us to fully define that sketch.
06:43
Let's undo this.
06:45
You can use control Z on the keyboard or you can use the undo option at the top.
06:49
And let's apply a dimension.
06:52
In this case, the dimension I want is going to be
06:56
one inch
06:57
and then I'm going to use some mathematical operators here plus a quarter inch
07:02
and we'll hit enter
07:03
what this allows us to do is drive the
07:05
diameter of the circle relative to other dimensions.
07:08
In the sketch.
07:09
For example, if I were to change this one inch value to 1.25 or two inches,
07:15
then you can see the overall sketches updated,
07:18
the rectangle updated as well as this large circle.
07:21
If I take this back down to one inch, you can see that everything changes as well.
07:26
So it's important to think about how your sketches are going to update.
07:30
If you always want this circle to be coincident
07:33
or intersect with the corner point of a rectangle,
07:35
then using a constraint is the best way.
07:38
However,
07:38
if you want the circle's diameter to be relative
07:41
to some other value or dimension in your sketch,
07:44
then making some sort of mathematical operator or equation allowing
07:48
you to drive that makes a little bit more sense
07:51
at any point in time we can change or
07:53
delete the constraints and dimensions in our sketch.
07:56
For example, I can select this and hit delete on the keyboard to get rid of it.
08:01
Then I can decide that I want to use that coincident constraint. After all,
08:05
if we have a coincident constraint or some other constraint,
08:08
and we decide that we don't want to use that,
08:10
we can always go back and change that as well.
08:12
Let's hit escape to get off our constraint tool and let's find
08:16
and select the parallel constraint that was added to our vertical line
08:20
with it selected,
08:21
it'll highlight the other constraint as well as the sketch geometry.
08:24
We simply need to hit delete on the keyboard
08:27
and now we can move this geometry around.
08:30
However, in this instance,
08:31
you'll note now the vertical constraint is likely
08:34
not the right constraint for the job.
08:36
So we're gonna select and delete the vertical constraint.
08:40
Now we want to use coincident between this line and this center point.
08:45
And while there's not a situation where those can touch
08:48
using the coincident constraint in this instance,
08:50
will allow us to take the extension of this line and make
08:53
sure that it always intersects the center point of that circle.
08:56
We can hit escape on the keyboard
08:58
and now we can drag this around to other positions.
09:01
So this is a great instance where using a constraint as well
09:04
as some dimensions to dictate a new position makes the most sense
09:09
if I needed that new feature to be at 60 degrees.
09:12
Now, I have a way that I can control it with both dimensions as well as constraints.
09:17
In some cases, you'll have all the information you need inside of a single sketch.
09:22
But in other instances, you may find that you need to go to your project,
09:25
include tools and project geometry from some other reference in your design.
09:30
In most cases, the project tool is used to gather information about your design.
09:34
For example, the inside diameter of this lower edge,
09:38
we're gonna say OK, and go back to our top view.
09:42
Notice that the projected geometry comes in as purple.
09:45
I'm gonna temporarily hide the body to make this a little bit easier to see.
09:49
This is a great way for us to bring in additional references.
09:53
And if they're not needed for sketch profiles,
09:55
we can select them and convert them to construction.
09:58
This means that they won't participate in the selection of those features.
10:02
For example, if this inside section isn't needed for our extrude,
10:07
we can select this curve
10:09
and make it construction.
10:11
This means that our only valid profile selections are now going to be inside of
10:14
this circle as well as the circle and rectangle in the center of our design.
10:20
We can also double click on sketch entities to get an entire profile.
10:24
And in this case, convert that to construction,
10:27
this allows us to have the geometry we need easily as well
10:30
as all the reference geometry to help drive the overall dimensions.
10:34
Understanding how a sketch is going to influence your design downstream,
10:38
takes a lot of practice and trial and error.
10:40
Once you have enough time using fusion and creating your own sketches,
10:45
you'll begin to understand how these initial decisions
10:47
on creating sketches will have a downstream effect.
10:51
But the good news is you can always go back to
10:53
these sketches at any point in time and make adjustments.
10:56
For example, I can double click on the original sketch used to drive this design
10:60
and I can make a change here.
11:02
If I make a change here, it's going to affect the overall design,
11:06
including the solid body and any additional geometry.
11:10
We can see that the position of this circle has updated
11:13
and we can make those changes once more by right clicking and showing the dimensions
11:20
and then making the change on the screen. So we can see the updates happen
11:24
playing around with simple designs is a great way to better understand the
11:27
limits and the constraints placed on your designs by these initial sketches.
11:31
So make sure that you spend enough time
11:33
getting comfortable with creating some basic sketch elements,
11:36
make sure that you apply dimensions and constraints
11:39
and come up with some examples of your own to figure out how to best use these.
11:43
Once you're done, let's go ahead and move on to the next step.
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