[♪ Music Playing ♪] Hey guys, it's Alex with Engineering
Applied. In this video, we're going to be taking a
look at the available 2D sketch constraint tools available in Autodesk
Inventor. If you're looking for a particular
function, check the description for time stamps. And if you don't find what you're
looking for in this video, go check out my other videos in my Autodesk Inventor
Tutorial Series because I'm confident you'll find exactly what you need.
Also, don't forget to like this video, subscribe to the channel, and turn on
notifications so you don't miss out on any helpful content like this in the
future. Let's get started. Okay, so to get started here, we're going
to be taking a look at our "dimension tool". And I have a few shapes
drawn up here because I want to show you the various dimensions that
this one tool can create for us. So starting here on the left, we have a
circle. So if we just click "Dimension" and then click on the outer
profile of the circle, we can constrain its diameter. So let's
constrain this to a quarter of an inch or we can also
constrain its location to a interest point, or a reference point.
So in this case, I want to use the origin. So I still have "Dimension" preselected.
So I'll just select the center of the circle. And then
I'm going to select this origin here and you can see we
could set the vertical distance or we could set the horizontal distance to
the origin. So we'll go ahead and just leave that as is and then we'll go ahead
and set a horizontal distance. Okay,
so now our circle is fully constrained. Next,
we can do a couple of things with lines within a profile. So here I have a
rectangle drawn up. We can either give a length to a leg
of a profile. So in this case we can set the length of this vertical leg.
So we could set that to, whoops, we could set that to 0.4
or we could set a distance. So what we could do is we could set the distance
between this horizontal leg and this horizontal
leg and it'll give us the same effect. However, we picked up two separate
segments to do this. So that's the difference: the first
option that I did here on the left that was a length,
this next way of dimensioning is a distance.
Okay, next we can also set an angle. So what we can do is we
make sure "Dimension" is toggled, and then we can come over to this shape
over here and we'll just set the angle between these two
lines. So say I want to set it to 35 degrees,
I can do that. Additionally, we can also pick up endpoints of a line. So if I
were to draw a line out in space somewhere here. I could
actually go to "Dimension", pick up the two end points,
and then it'll give me a distance there between the two endpoints. The next
constrain tool we have is the "Auto Constrain" tool. And so in
this particular case I have a rectangle drawn up somewhere out in
space and then I also have a point fixed at the origin.
So what we can do here is we can auto constrain a profile that's found in our
sketch plane. So, we click auto constrain and then if you
look in this dialog box we have our first option which is our
curve selection tool. So we'll just select the curves that we
want to auto dimension and constrain. You'll notice we have two check boxes
here: one is to make sure that we're auto dimensioning and one is
to make sure we're applying constraints. And you'll see that, "hey we have four
dimensions required to fully define the shape".
Now, what you'll notice is if I hit "Apply", it'll add the vertical and the
horizontal leg lengths but it's still blue and it says
we still need two dimensions. That's because this is still free floating in
space. So if I click "Done", I can still click it and move it in the
vertical direction and I can still click and move it in the horizontal direction.
So if you're ever unsure if something is not constrained fully or
in which direction it's not constrained in, just grab your profile and click and
drag it somewhere and that'll give you some insight
into what needs to be constrained. So let's go ahead, we're going to undo this,
and we're going to highlight auto constrain again.
We're going to pick up the profile, but we're also going to pick up
the point here. And let's say this is where we want the rectangle to stay,
out in space. So we've got all of our reference geometry and our actual
geometry selected. We click "Apply", and now you'll notice that our rectangle
is black. And that means that everything is
fully defined in this sketch. So we have our vertical dimension, our horizontal
dimension, and then we have our actual location of the rectangle out in space
defined as well. Now we can actually go back and re-dimension things as
necessary. So I could change that to 0.4, if I wanted
to say. So now we have a fully dimensioned
rectangle out in space and that's how you use the auto dimension and constrain
tool. The next function is the "Show
Constraints" button. And so what this basically does,
is it shows us all of the applied constraints that are found in
our sketch geometry. So if I click this, and then highlight everything, you'll
notice that in these shapes I have drawn up, it tells me what constraints are
being applied to these profiles. So starting on the left here, I have an
arc that is constrained as concentric to this circle. So basically
it means that the center point of this arc
is coincident with the center point of the circle. Now moving over to the right,
we have a rectangle and you'll notice these little two lines that are moving
up at an angle side by side. This is the "Parallel
Constraint" and you'll also notice that you have
these two lines horizontal, that basically says that, "hey
this is a horizontal constraint". And lastly, you have this perpendicular
constraint at the corner. So with all of these constraints applied,
this tells the rectangle that, "hey I have two vertical legs, two horizontal
legs, and then everything is 90 degrees from one another".
If we want to hide the constraints that we've shown, we can highlight everything,
right click and go down to "hide all constraints". And you'll see the
shortcut here once you have this menu open is "F9". So we could just click
"hide all constraints" and then there we go.
Now all the constraints are hidden again, we can freely grab the corners,
the endpoints of our profiles, and manipulate it
as needed. Next, we have our "Constraint Settings Menu". So if we go into this menu,
we can play around with our constraint settings, change our inference
settings, and enable and disable relax mode and
then edit what gets removed when we enable this
mode. So, what relax mode does, is if we go to this
fully defined rectangle and we try to click and drag the lines,
it doesn't move because it's already fully defined,
there's no movement left in this. So what we can do is we can go to "Constraint Settings", relax mode and enable it, and these
features that I have checked off here will be removed
in this mode. And So when I go to this rectangle and click and drag again,
it removes those constraints. So like the horizontal constraint and some of the
parallel constraints, and then I can click and drag this and move it wherever
I want. And then it removes them all together
when I'm done. Okay now we're getting into the
individual constraints themselves. So the first one we're taking a look at here is
the "Coincident Constraint". So in this case, let's say I've already
dimensioned the diameter of my circle and I want to set the center point of
the circle coincident with the origin. So what I can do, is I
can click my "coincident constraint". And then
I can go to the center point of the circle,
click that once, and since I want to constrain it to the
center point of the origin, I can go to the origin drop down folder
here in my model tree, and I could just go to center point and left
click on that. And then it'll snap it to the origin itself and now you
see we're fully defined. We can also manually put down a point. So
what I'll do is I'll just undo that and I'll just manually
put a point somewhere in space. And let's say I'll just go ahead and fix
this here because that's where I want it. And then I can go back to "coincident",
click on the center point, and then click on the point and then
it'll snap it to that area. Another example for the coincident constraint is,
say in this case, I want the endpoint of this line to be coincident with this
line. I just have to click "coincident" there. I
can click on the endpoint and then I can click on the line itself and it will
drop it there. Now we're at our parallel constraint. So
in this particular case, I've drawn up a shape
somewhere out here in space. And I want this angled line
to be parallel to this line that I've constrained here and we'll actually go
ahead and make this a construction line. So what we can do is we can click
"parallel", click the first line, and then click this
line and it'll set the two parallel. What we can also do too, is I can
pre-select the two lines first by holding down CTRL and then clicking
both of them, making sure they're both selected. And then I can go to "parallel
constraint", and then click that and it'll apply the constraint as well.
Now for our tangent constraint, in this particular case I want to set
this line tangent to the circle. So I went ahead and fixed the line out
here in space so that the circle will move to it.
So what we'll do is we'll go ahead and click "tangent". Click
either the line or the circle, it doesn't matter. So we can click the line first
and then the circle or we can go back and click the circle
first and then the line. And then that sets the circle tangent to
that line. Okay, so the next tool is the "Collinear
Constraint". And so the "collinear constraint", all this
does, is it sets two line segments collinear. Which basically means that
it's on the same line. So if two lines are out in space, I
can bring one down to be collinear with the other.
So here I have an example of a shaft that I want to revolve around
the X-axis. Before I revolve this, I need to set a constraint so that this
is collinear with this regardless of whatever dimension or height
I make this here. So basically all I have to do is go to "collinear",
click on the one segment, click on another segment, and then it sets it
collinear and then now I'm defined in that direction.
And you'll notice if I change this dimension here, let's say we change it to
0.425, this line travels with it. And this is a good practice to make your
design more efficient. Next we have our "Perpendicular
Constraint". This is very simple. So basically this sets two line segments
within whatever profile you have drawn up in your sketch
plane to be 90 degrees from one another. So let's just say
we're drawing some sort of set of line segments. It doesn't matter
what length they are for this particular example. I just want these two line
segments to always be 90 degrees with respect to one another. So I just go
to "perpendicular", and then click this line, and then click
that line, and then it sets it 90 degrees to one another there. Next, we have our
"Smooth "Constraint". And so for this constraint, I set up two
horizontal lines and then an interpolated spline between
the two with a single somewhat middle point, it's
not perfectly middle to the arc but it's not important for this case.
So what I do is I go to "smooth", I click on this line and then
the spline. And you'll see it sets the end,
or I should say the beginning, of this spline here
in line with that first line. But you'll notice down here,
we're still going in at an odd angle with reference to this line. So what
we'll go ahead and do is we'll go ahead and click on the curve, and then click
the line that we want to smooth it to, and then there we go it smoothes out
that spline to be in line at the end points with this
geometry that was previously drawn up. Next, we have the concentric constraint.
And so what we could do with this, is we could set two circular elements
concentric to one another; meaning that their center points will be
coincident. So in this case, I have a profile drawn up
where I performed a fillet on
these two top corners up here and I just want to constrain
this circle concentric to this arc here. So I'll just press this
"concentric constraint" button up here, select the circle,
and then select the arc. And you'll see that it snaps the circle
concentric to that arc there and I can use this to
perform a cut through the part or whatever it is that I'm doing
here. Okay, next, I'm going to bundle in the
horizontal and the vertical constraints together. So I have a profile
drawn up here; there's no particular rhyme or reason to the angles
or anything like that. But essentially, I want to create
a rectangle out of these random lines that are on the screen here. So
the first thing I need to do is I need to set the top and the bottom legs
horizontal. So what I'll do is I'll go to the horizontal constraint,
I'll click this line, it'll set the top line horizontal. I'll do the same for the
bottom, and there it goes it sets that
horizontal as well. Then, I'll go to the vertical,
and I'll just set that vertical and that one vertical, and now I have my rectangle.
Okay so next we have our "Symmetric Constraint". So in this case I have
three separate line segments but they're all joined by a single point.
And this angle inside here is different from this angle. This angle
is larger, and what I want to do is I want to create some
symmetry around this vertical line. So I want this angle and this angle to be
the same, and the whole thing symmetrical. So what
I can do is I can click "symmetric". I'll select one leg
and then I'll select the second leg that I actually want to change
for the symmetry. And then I'll select the third line in which I want to make
this whole thing symmetric to. And then there we go. Now we have a
symmetric shape and then we could go back and
you know, dimension these line lengths or whatever else we got to do there.
Okay, so next we have our "Fix Constraint". So the "fix
constraint" is extremely simple to use. So all you do is you click the
little lock icon here for "fix" and then we just click
all of the sketch elements that we want to fix in space. So we could click
anything from rectangular shapes, to circles, to line
elements, whatever it is that we have there
and you'll see it locks them into place. And now if I go to click and drag these,
they're not going anywhere. So this is helpful if you're drawing up
a concept real quick, you're not really interested
in dimensioning the whole thing, you just need to lock something in space real
quick like a little point or something like that,
this can be useful for that. Okay so we have our "Equal Constraint" here. And so
what this does is it sets various types of dimensions equal to one another
depending on the scenario. So in this case,
I have a rectangular profile, and the first thing I want to do with this is I
want to set all of the circles equal to one another.
So I have the first one dimension to one inch in diameter. So I'll go to "equal",
I'll select the first circle, and then just start
selecting the first circle and then the subsequent circles that I want to match
to it. So, I've got that one done, I can go down
here and lastly get this last one. And now, you'll notice that I've drawn
a line segment from each corner to the center point of each circle and I
want to set these line segments equal. So what I'll go ahead and do, is I'll set
a dimension for these lines here. So I'll just go ahead and set this one to
whatever it happens to be. And then I'll set all these other line
segments equal to that. So I'll click the first line and then
click this line, and then go through and do that for the
rest of them here. Picked up the wrong line there. If you're
having trouble picking up a particular profile you can
hover the mouse over the general area of what you're trying to get,
and then a little drop down will pop up like this, you can go to the drop down
here and then it'll highlight whatever it is
that you can select. So I'm going to go down to this number two option.
And now I've got that curve and now I can set it equal to that.
And then lastly, we could do this one, and there we go. Now we have all of our
little line segments set to the same dimension. And you could apply
this in all sorts of scenarios. This is really useful
for boosting the efficiency of your design. So that, let's say for example, I
want to change one diameter and not four diameters, I
can do that. So I can just double click on this and say I wanted to change it to
1.25. It changes everything all at one time.
Okay, so our next constrain tool is our "Edit Coordinate
System", and to get here you just pull this
little drop down menu open, and you can tell there's a drop
down menu there by that little arrow, and you click "edit coordinate system". And
you'll notice I created a 3D body
of just some arbitrary shape because what we can do
is we can edit the native coordinate system found
when creating a sketch on a plane. So in this case, I'm creating a sketch on this
plane. So if we look normal to that, we see this
is our default origin location and you can see the axis
coincides with this one point on the vertex here of the shape.
But, let's say I want to move the origin up to this point up here. What we could
do is we can click and hold on that point, and then we can drag it up
until it stops. And what you'll notice is once we double
click there, the axis is now frozen here.
To validate this all we do is right click and go to "Ok",
or you can press the enter key, and now you notice that the origin has shifted
up to that point that we told it to. Now if we undo that,
we can go back down and we can also do another type of
translation of the coordinate system. So we go back to "edit coordinate system",
and let's say I want to change the X axis
to be in line with this angle here. So what I do is I click the little red
leg, which is the X-axis, and then click this part feature here
on this angle. So we'll click that and now you'll notice the X-axis is in line
with that and then if we go to "Ok", the coordinate system has shifted to now
be in line with that. So this is really
handy if you're trying to create some eccentric geometry that is referenced off
a different set of origin directions. Okay, so the final tool that
we're going to be taking a look at in the session is the
"Constraint Inference Scope". And so what this allows us to do is it allows us to
control what geometry is used to infer constraints when creating new
geometry. So what does this mean? Well, when we open
this command, we see three options here. By default,
it has the geometry and current command selected. So,
what we're going to go ahead and do is I'll start out by drawing a couple of
lines. So we'll just set the first down, first one down it doesn't matter
where, and then we'll go to create a second line and I want you to pay
attention to where the cursor snaps and what
constraints do or do not pop up when I use this. So
I'll start the first end point here, and we'll get to the end, and you'll
notice that it snaps to the end but
no parallel constraint is automatically inferred here. So just remember that.
So if I go back and grab my endpoint, I can move my line and
it, there's no parallel constraint inferred there. So I'll just click "undo".
But, next what I'll do is I'll go back to "constraint inference scope",
select "all geometry", and press "Ok". Now when I create a line,
and we'll reference it off this top one, you see it wants to snap to the end
point. We'll let it. And then you, you already see down here
in the middle, as I'm dragging this line down, it infers
a parallel constraint automatically. And I can do that with any geometry
found in the sketch plane because I allow it to.
So if I drop that line, you'll see that it's automatically inferred
that, that constraint there. And so, you see that these two lines
don't have it but these two do and if I move this, this other line moves
with it. The final option within our "constraint inference scope" menu is
the "select" option. And so to illustrate this what I'm going
to do first, is I'm going to draw a line that's not quite parallel with these two
lines here, but close. And I want to show you that I
can infer constraints specifically off of
whatever selected geometry I choose and nothing else in the sketch
plane. So I'll just drop this line somewhere in here
and get it close to the angle but don't let it snap to anything else.
Okay, so now I go back to my "inference scope menu",
go to "select", and I only want to infer constraints off of this line.
I select that line, it turns light blue, I'll hit "Ok", and now it turns dark purple.
It may be a little tough to see on screen but when you do this on your own
computer you'll see that it changes colors to indicate that this is the
targeted geometry for our inference. So, now we have that selected. We'll go back
to our line tool, and even if I come out here just into
space and get that to snap to the other line,
it's not going to let me infer any sort of constraints like our parallel
constraint with these two lines. But you'll notice
it lets me infer that parallel constraint with that originally
selected line that's now in that dark purple color.
So we can drop it there and there you go. It's
now constrained as parallel and we've completed that option.
That concludes this segment of the Autodesk Inventor Part Creation Module
where we took a look at the available 2D sketch constraints.
Don't forget to like this video, subscribe to the channel, and turn on
notifications to stay up to date on future content as it's released. And as
always, don't hesitate to reach out and let me
know if there's anything else you'd like to learn about or see on this channel.
I genuinely appreciate you watching and learning from me
and I can't wait to make more helpful content like this for you in the future.
Thanks for watching, and I'll see you again soon! [♪ Music Playing ♪]
