& Construction

Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
& Manufacturing

Professional CAD/CAM tools built on Inventor and AutoCAD
Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
Professional CAD/CAM tools built on Inventor and AutoCAD
Transcript
00:02
foundational CAD concepts
00:06
in this video. We'll understand basic sketch creation.
00:09
We use dimensions and constraints to define a sketch and will create a three D.
00:14
Model using basic tools
00:17
infusion 3 60. We want to get started with a new untitled document.
00:21
The first thing that we're gonna do is we're
00:23
going to check our document settings and make sure
00:25
that the units are going to be what we want to use to design our parts for me.
00:29
I'm going to change the unit type two inch and say, okay,
00:33
note that if you're constantly using the inch unit system,
00:36
you can't set that as your default either when
00:38
you're changing the document settings or you can go up
00:41
into your user preferences and you can set up
00:43
your units for your design and your manufacturer workspace.
00:47
So you'll notice that there's a section called unit values and displays.
00:51
And then we also have default units. So in the design
00:55
and the manufacture section,
00:56
you can set those to whatever you constantly use for us.
00:60
I'm going to do it on a per document basis.
01:03
Now that we have our unit set,
01:04
we're going to start creating a design by first creating a sketch.
01:07
A sketch is going to be the basis of any of our parametric designs.
01:11
We get started by selecting create sketch and then
01:14
we can pick one of the default planes.
01:16
Front top or right
01:19
now in this case,
01:20
I'm going to select the front plane which is my
01:22
XZ plane because we're working in the Z up orientation.
01:26
The first thing that I want to do is take a
01:28
look at my sketch pallet on the right hand side.
01:30
Whenever we're inside of a sketch, new tools are presented to us.
01:34
The sketch palette is a good way for us to change some
01:37
of the visualization options such as
01:38
showing or hiding dimensions and constraints.
01:41
We also have a whole host of new tools that are displayed at the top on this sketch tap.
01:47
Now inside of here we have our create tools are modified tools,
01:51
a section for constraints and then we have some
01:53
additional tools that pop up on many different menus.
01:56
First we want to look at creating some sketch entities.
01:60
These can be lines, rectangles, circles and so on for our design.
02:04
We're going to get started using the line tool so
02:06
we can understand how dimensions and constraints work First.
02:10
When I select the line tool, I'm going to begin by selecting the origin
02:14
as the cursor gets closer to the origin. Notice that it snaps
02:18
by default snaps are going to be enabled to certain geometry such as the origin.
02:23
However, the rest of our sketch doesn't have any snaps turned on.
02:28
If you're familiar with working with snaps,
02:30
you can go to your grids and snap settings and turn on snap to grid.
02:34
This will allow you to snap to each incremental intersection point in your grid.
02:38
For this example, I'm going to leave that turned off and just snap to the origin.
02:42
Also notice that as I'm moving my cursor around,
02:45
it's displaying the dimension on the screen in blue
02:48
as well as the angle from my horizontal.
02:51
These are also options that you can turn
02:52
on or off inside of your general user preferences
02:56
for me.
02:57
I'm going to drag this line close to vertical and as soon as I get there you
03:00
can see that it's snapping to vertical and a
03:03
blue icon is displayed representing a vertical constraint.
03:06
I'm going to left click to place that line
03:09
and I'm going to begin dragging out to the right
03:12
while we're dragging out to the right.
03:14
If we don't enter any values for the dimension or the angle they will not be created.
03:19
But notice that it is adding another constraint at the
03:22
intersection point and that's going to represent a perpendicular constraint.
03:27
If we want to specify a certain distance and angle
03:31
we can do that by manually entering the value.
03:33
For example three I can hit tab to go over
03:37
to my angle dimension and hit 85 can hit enter and
03:41
that will accept those values and end the line tool notice
03:44
that this line is blue while this one is black,
03:47
black sketch entities means they're fully defined
03:51
while blue means they're under defined.
03:53
Now it's a little bit misleading because this line here is
03:57
not fully defined because its endpoint can still move vertically,
04:01
we can see that by just left clicking on this
04:03
endpoint holding down the mouse button and moving it around
04:06
this line here
04:08
is three inches long
04:09
and at 85 degrees.
04:11
So in order to fully define its position,
04:13
we need to give a dimension to this vertical line.
04:16
Let's go ahead and navigate back to our dimension tool.
04:19
We find this under the create menu under sketch dimension.
04:22
You can also expand the menu and go all the way to the bottom
04:25
and note that D on the keyboard is the shortcut for sketch dimension.
04:30
We're going to select this line and now we're placing a vertical dimension.
04:34
Well left click and then we can enter a value of 2.5 in
04:38
now, all of our sketch entities are currently fully defined.
04:42
Let's go ahead and hit escape on the keyboard to get off our dimension tool.
04:46
And once again, let's use the line tool.
04:48
This time I'm going to draw two lions just out in space,
04:51
making sure that they don't snap to any specific constraint.
04:55
If you do have to draw a line or some sketch entity that's close to a constraint,
04:59
you don't want to snap.
05:00
You can hold down the control key on the pc or the
05:03
command key on a Mac to temporarily override those persistent constraints.
05:09
Once we've placed those two lines, we can either hit escape on the keyboard,
05:12
the green,
05:13
check mark that displays or we can right click and select OK from the marking menu.
05:18
Now that we have these two lines created.
05:20
Note that they are under defined but they do have a constraint in the corner.
05:24
This is a coincident constraint.
05:26
What I'd like to do is I'd like to
05:28
create a perpendicular constraint between these two lines,
05:31
make sure that one of them is vertical or horizontal
05:34
and then connect them with the rest of our geometry.
05:36
So from our constraints menu we can select perpendicular constraint.
05:41
Then we can select the two entities.
05:43
Once we have perpendicular,
05:45
I'm going to navigate over and select horizontal vertical.
05:49
I want to make sure that this line is horizontal. Then I want to select coincident.
05:54
I'm going to take this endpoint and make it coincident with this one here.
05:58
I'm going to hit escape to get off of
06:00
the coincident tool and I'm just going to simply drag
06:03
this endpoint around and note that we can drag
06:05
it to a position where it is also coincident.
06:08
So you can manually drag these points around or
06:11
you can use your constraints to attach them.
06:14
Another thing that's important to note if we were to sketch another line
06:19
and if we right click on it after it's selected
06:22
the constraints that are applicable will show in the right click menu.
06:26
So fixed.
06:27
Unfixed, will lock it in its current position,
06:29
horizontal vertical will allow us to create either a horizontal or vertical line
06:33
and delete coincident will allow us
06:36
to delete any constraint that's currently applied
06:38
in this case a coincident constraint.
06:41
I don't need this line so I'm going to select it and hit delete on the keyboard.
06:46
Now we have a complete closed profile and we can tell because the sketch grid
06:51
is displayed in white but inside of this area we have a selectable region.
06:56
This is called our sketch profile.
06:58
We can turn on and off the profile but this lets us know
07:02
that we have something that's applicable for something like a solid extrude.
07:06
We can also use an open profile for thin wall extrude but
07:10
we're not going to be talking about that in this video.
07:13
The last thing that I want to do before we move on is I
07:15
want to place a hole or a circle directly in the middle here.
07:20
In order to do that. We need to add some construction geometry.
07:23
There are a couple of different ways that we can do this.
07:26
The line types that we want to use will be construction and they
07:28
can either be applied after the fact or before we start sketching.
07:32
Let's take a look at both.
07:33
First we're going to select the line tool and
07:36
I'm going to go from this bottom left corner to
07:38
the upper right hand corner and then I'm going to hit escape to get off my line tool.
07:42
This line currently divides our profile into giving us two selectable regions.
07:47
I only want this to be a construction line. So I'm going to select it.
07:51
Go over to my line types and click on construction.
07:54
There's also a default shortcut key
07:57
X. On the keyboard.
07:59
Another way that we can do this is we
08:00
can pre define construction geometry before we get started.
08:04
So now if I select the line tool and I begin sketching from the opposite corner
08:08
that is automatically created as construction geometry.
08:12
If I hit escape notice that this is still construction,
08:16
there is a center line option and this
08:18
is extremely helpful when making revolved parts,
08:21
it will automatically turn dimensions to
08:23
the center line into diameter dimensions.
08:26
And it also works just like a construction line because
08:29
it's not able to be selected for solid features.
08:32
Now that we have this closed region, let's go ahead and use a center diameter circle.
08:37
I'm going to place the center diameter circle directly on one of these lines.
08:42
I'm going to hit escape to get off my circle tool and notice that
08:46
this is fixed to our line and can be dragged back and forth.
08:49
There is a point on this line that actually has a midpoint,
08:53
but because we're not dealing with a true rectangle or square,
08:56
its midpoint is not going to be the intersection of this other line.
08:59
So what we want to do is we want to make sure that the center point
09:02
of the circle is also coincident with this line which will give us our intersection.
09:07
So we're going to use the coincident constraint,
09:09
select the center point of our circle,
09:11
our construction line and now they're snapped together.
09:15
Now I want to apply a sketch dimension to represent the diameter of this whole.
09:20
I'm gonna make this 1.25" and hit enter.
09:24
Let's go ahead and finish the sketch.
09:26
Go to our create menu and select extrude.
09:29
Select the closed profile region that we want
09:32
to extrude and begin dragging this out.
09:34
Note that there are several options inside of the extra dialogue box for example,
09:38
symmetric
09:40
since we did base this about the front plane,
09:42
it is helpful for us to use symmetry and that will
09:45
help us later on when we're trying to plan out manufacturing.
09:49
Once we're done we can enter the distance 1.5 in we can determine
09:53
whether or not that's for the half segment or the overall length.
09:57
And then we can say, Okay,
09:59
now that we have solid geometry,
10:01
we can use modified tools such as Philips or champers.
10:04
If I select Philip
10:05
and I select corners, I can use the
10:08
tool to round those off. I'm going to right click and say okay,
10:12
and then I'm going to use my right click marking menu to repeat the, fill it again
10:16
this time.
10:16
Notice that it's grabbing the entire chain because the tangent c added from
10:21
those other filets allows us to go all the way around these corners.
10:24
We can turn tangent chain off which will only make use of the selected edges.
10:30
Now that we've made a basic design. Let's go ahead and save it.
10:34
We're going to use the save option.
10:36
It will automatically be placed in our project that we're currently working in
10:40
and I'm going to call this intro to CAD and hit enter.
10:45
At this point,
10:46
I strongly suggest that you play around with additional sketching
10:49
tools as well as some basic creation and modification tools
10:53
and once you're ready,
10:54
go ahead and save your design and then we can move on to the next step.
Video transcript
00:02
foundational CAD concepts
00:06
in this video. We'll understand basic sketch creation.
00:09
We use dimensions and constraints to define a sketch and will create a three D.
00:14
Model using basic tools
00:17
infusion 3 60. We want to get started with a new untitled document.
00:21
The first thing that we're gonna do is we're
00:23
going to check our document settings and make sure
00:25
that the units are going to be what we want to use to design our parts for me.
00:29
I'm going to change the unit type two inch and say, okay,
00:33
note that if you're constantly using the inch unit system,
00:36
you can't set that as your default either when
00:38
you're changing the document settings or you can go up
00:41
into your user preferences and you can set up
00:43
your units for your design and your manufacturer workspace.
00:47
So you'll notice that there's a section called unit values and displays.
00:51
And then we also have default units. So in the design
00:55
and the manufacture section,
00:56
you can set those to whatever you constantly use for us.
00:60
I'm going to do it on a per document basis.
01:03
Now that we have our unit set,
01:04
we're going to start creating a design by first creating a sketch.
01:07
A sketch is going to be the basis of any of our parametric designs.
01:11
We get started by selecting create sketch and then
01:14
we can pick one of the default planes.
01:16
Front top or right
01:19
now in this case,
01:20
I'm going to select the front plane which is my
01:22
XZ plane because we're working in the Z up orientation.
01:26
The first thing that I want to do is take a
01:28
look at my sketch pallet on the right hand side.
01:30
Whenever we're inside of a sketch, new tools are presented to us.
01:34
The sketch palette is a good way for us to change some
01:37
of the visualization options such as
01:38
showing or hiding dimensions and constraints.
01:41
We also have a whole host of new tools that are displayed at the top on this sketch tap.
01:47
Now inside of here we have our create tools are modified tools,
01:51
a section for constraints and then we have some
01:53
additional tools that pop up on many different menus.
01:56
First we want to look at creating some sketch entities.
01:60
These can be lines, rectangles, circles and so on for our design.
02:04
We're going to get started using the line tool so
02:06
we can understand how dimensions and constraints work First.
02:10
When I select the line tool, I'm going to begin by selecting the origin
02:14
as the cursor gets closer to the origin. Notice that it snaps
02:18
by default snaps are going to be enabled to certain geometry such as the origin.
02:23
However, the rest of our sketch doesn't have any snaps turned on.
02:28
If you're familiar with working with snaps,
02:30
you can go to your grids and snap settings and turn on snap to grid.
02:34
This will allow you to snap to each incremental intersection point in your grid.
02:38
For this example, I'm going to leave that turned off and just snap to the origin.
02:42
Also notice that as I'm moving my cursor around,
02:45
it's displaying the dimension on the screen in blue
02:48
as well as the angle from my horizontal.
02:51
These are also options that you can turn
02:52
on or off inside of your general user preferences
02:56
for me.
02:57
I'm going to drag this line close to vertical and as soon as I get there you
03:00
can see that it's snapping to vertical and a
03:03
blue icon is displayed representing a vertical constraint.
03:06
I'm going to left click to place that line
03:09
and I'm going to begin dragging out to the right
03:12
while we're dragging out to the right.
03:14
If we don't enter any values for the dimension or the angle they will not be created.
03:19
But notice that it is adding another constraint at the
03:22
intersection point and that's going to represent a perpendicular constraint.
03:27
If we want to specify a certain distance and angle
03:31
we can do that by manually entering the value.
03:33
For example three I can hit tab to go over
03:37
to my angle dimension and hit 85 can hit enter and
03:41
that will accept those values and end the line tool notice
03:44
that this line is blue while this one is black,
03:47
black sketch entities means they're fully defined
03:51
while blue means they're under defined.
03:53
Now it's a little bit misleading because this line here is
03:57
not fully defined because its endpoint can still move vertically,
04:01
we can see that by just left clicking on this
04:03
endpoint holding down the mouse button and moving it around
04:06
this line here
04:08
is three inches long
04:09
and at 85 degrees.
04:11
So in order to fully define its position,
04:13
we need to give a dimension to this vertical line.
04:16
Let's go ahead and navigate back to our dimension tool.
04:19
We find this under the create menu under sketch dimension.
04:22
You can also expand the menu and go all the way to the bottom
04:25
and note that D on the keyboard is the shortcut for sketch dimension.
04:30
We're going to select this line and now we're placing a vertical dimension.
04:34
Well left click and then we can enter a value of 2.5 in
04:38
now, all of our sketch entities are currently fully defined.
04:42
Let's go ahead and hit escape on the keyboard to get off our dimension tool.
04:46
And once again, let's use the line tool.
04:48
This time I'm going to draw two lions just out in space,
04:51
making sure that they don't snap to any specific constraint.
04:55
If you do have to draw a line or some sketch entity that's close to a constraint,
04:59
you don't want to snap.
05:00
You can hold down the control key on the pc or the
05:03
command key on a Mac to temporarily override those persistent constraints.
05:09
Once we've placed those two lines, we can either hit escape on the keyboard,
05:12
the green,
05:13
check mark that displays or we can right click and select OK from the marking menu.
05:18
Now that we have these two lines created.
05:20
Note that they are under defined but they do have a constraint in the corner.
05:24
This is a coincident constraint.
05:26
What I'd like to do is I'd like to
05:28
create a perpendicular constraint between these two lines,
05:31
make sure that one of them is vertical or horizontal
05:34
and then connect them with the rest of our geometry.
05:36
So from our constraints menu we can select perpendicular constraint.
05:41
Then we can select the two entities.
05:43
Once we have perpendicular,
05:45
I'm going to navigate over and select horizontal vertical.
05:49
I want to make sure that this line is horizontal. Then I want to select coincident.
05:54
I'm going to take this endpoint and make it coincident with this one here.
05:58
I'm going to hit escape to get off of
06:00
the coincident tool and I'm just going to simply drag
06:03
this endpoint around and note that we can drag
06:05
it to a position where it is also coincident.
06:08
So you can manually drag these points around or
06:11
you can use your constraints to attach them.
06:14
Another thing that's important to note if we were to sketch another line
06:19
and if we right click on it after it's selected
06:22
the constraints that are applicable will show in the right click menu.
06:26
So fixed.
06:27
Unfixed, will lock it in its current position,
06:29
horizontal vertical will allow us to create either a horizontal or vertical line
06:33
and delete coincident will allow us
06:36
to delete any constraint that's currently applied
06:38
in this case a coincident constraint.
06:41
I don't need this line so I'm going to select it and hit delete on the keyboard.
06:46
Now we have a complete closed profile and we can tell because the sketch grid
06:51
is displayed in white but inside of this area we have a selectable region.
06:56
This is called our sketch profile.
06:58
We can turn on and off the profile but this lets us know
07:02
that we have something that's applicable for something like a solid extrude.
07:06
We can also use an open profile for thin wall extrude but
07:10
we're not going to be talking about that in this video.
07:13
The last thing that I want to do before we move on is I
07:15
want to place a hole or a circle directly in the middle here.
07:20
In order to do that. We need to add some construction geometry.
07:23
There are a couple of different ways that we can do this.
07:26
The line types that we want to use will be construction and they
07:28
can either be applied after the fact or before we start sketching.
07:32
Let's take a look at both.
07:33
First we're going to select the line tool and
07:36
I'm going to go from this bottom left corner to
07:38
the upper right hand corner and then I'm going to hit escape to get off my line tool.
07:42
This line currently divides our profile into giving us two selectable regions.
07:47
I only want this to be a construction line. So I'm going to select it.
07:51
Go over to my line types and click on construction.
07:54
There's also a default shortcut key
07:57
X. On the keyboard.
07:59
Another way that we can do this is we
08:00
can pre define construction geometry before we get started.
08:04
So now if I select the line tool and I begin sketching from the opposite corner
08:08
that is automatically created as construction geometry.
08:12
If I hit escape notice that this is still construction,
08:16
there is a center line option and this
08:18
is extremely helpful when making revolved parts,
08:21
it will automatically turn dimensions to
08:23
the center line into diameter dimensions.
08:26
And it also works just like a construction line because
08:29
it's not able to be selected for solid features.
08:32
Now that we have this closed region, let's go ahead and use a center diameter circle.
08:37
I'm going to place the center diameter circle directly on one of these lines.
08:42
I'm going to hit escape to get off my circle tool and notice that
08:46
this is fixed to our line and can be dragged back and forth.
08:49
There is a point on this line that actually has a midpoint,
08:53
but because we're not dealing with a true rectangle or square,
08:56
its midpoint is not going to be the intersection of this other line.
08:59
So what we want to do is we want to make sure that the center point
09:02
of the circle is also coincident with this line which will give us our intersection.
09:07
So we're going to use the coincident constraint,
09:09
select the center point of our circle,
09:11
our construction line and now they're snapped together.
09:15
Now I want to apply a sketch dimension to represent the diameter of this whole.
09:20
I'm gonna make this 1.25" and hit enter.
09:24
Let's go ahead and finish the sketch.
09:26
Go to our create menu and select extrude.
09:29
Select the closed profile region that we want
09:32
to extrude and begin dragging this out.
09:34
Note that there are several options inside of the extra dialogue box for example,
09:38
symmetric
09:40
since we did base this about the front plane,
09:42
it is helpful for us to use symmetry and that will
09:45
help us later on when we're trying to plan out manufacturing.
09:49
Once we're done we can enter the distance 1.5 in we can determine
09:53
whether or not that's for the half segment or the overall length.
09:57
And then we can say, Okay,
09:59
now that we have solid geometry,
10:01
we can use modified tools such as Philips or champers.
10:04
If I select Philip
10:05
and I select corners, I can use the
10:08
tool to round those off. I'm going to right click and say okay,
10:12
and then I'm going to use my right click marking menu to repeat the, fill it again
10:16
this time.
10:16
Notice that it's grabbing the entire chain because the tangent c added from
10:21
those other filets allows us to go all the way around these corners.
10:24
We can turn tangent chain off which will only make use of the selected edges.
10:30
Now that we've made a basic design. Let's go ahead and save it.
10:34
We're going to use the save option.
10:36
It will automatically be placed in our project that we're currently working in
10:40
and I'm going to call this intro to CAD and hit enter.
10:45
At this point,
10:46
I strongly suggest that you play around with additional sketching
10:49
tools as well as some basic creation and modification tools
10:53
and once you're ready,
10:54
go ahead and save your design and then we can move on to the next step.
Step-by-step guide
How to buy
Privacy | Do not sell or share my personal information | Cookie preferences | Report noncompliance | Terms of use | Legal | © 2025 Autodesk Inc. All rights reserved
Sign in to start learning
Sign in for unlimited free access to all learning content.Save your progress
Take assessments
Receive personalized recommendations
May we collect and use your data?
Learn more about the Third Party Services we use and our Privacy Statement.May we collect and use your data to tailor your experience?
Explore the benefits of a customized experience by managing your privacy settings for this site or visit our Privacy Statement to learn more about your options.