Design is the first phase in the digital manufacturing process. In this course, through a series of lectures and hands-on lessons, we’ll examine a designer’s approach to the design and manufacturing process—from concept to 3D model. We’ll start by applying design thinking to understand user needs, and then we’ll explore design criteria as we dive deeper into Autodesk® Fusion 360™ sketching, modeling, rendering, and documentation features.
Creating prop protection solid
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From the course by Autodesk
3D Model Creation with Autodesk Fusion 360
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From the lesson
2D Sketches to 3D Solid Model
This week expands on our layout sketches and begins to create a solid 3D model. Through the use of some basic and advanced features, we learn various tools of the trade to create complex 3D shapes. We also expand our Autodesk® Fusion 360™ knowledge and skills into the Patch workspace and explore how to add or remove solid geometry with surfaces.
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In this lesson, we'll start Creating a Prop Protection Solid.
After completing this lesson,
you'll be able to Create a Surface Extend,
Create a Split Body and Remove a Body.
The next step in our process is going to be to trim this geometry out.
There are three different ways that we can do this.
We can do it before we create a solid,
we can trim it as a surface,
or we could thicken it and then trim it as a solid.
And either method is going to be fine.
You will get some varying results that we want to talk about though.
Now remember, when you use a "thicken" operation,
what you're actually doing is you're taking the material,
the surface that we're working with and you're taking it out normal to the curvature.
So the first thing I want to do in this case is I'm actually going
to extend both of these edges out a
little bit and the reason I want to do that is because when I thicken this,
I want to make sure that I have enough material to cut.
So there are two options that we can use here, "Natural" and "Tangent".
Now you'll notice that "Tangent" doesn't work in this case but "Natural" does,
and there's no division on the surface,
so it's going to give us a nice smooth curvature transfer.
So we're going to go ahead and say "okay."
Now the distance ultimately doesn't matter as long
as we're extending out far enough for us to trim it,
and you can see it's rolling over a little bit in this corner.
But we're starting our trim from here.
So again, that doesn't really affect what we're doing.
But now what we're going to do is we're going to show sketch six,
and I'm going to go ahead and rename sketch six while I'm at
it and call this "Landing Gear."
And what we want to do is, we want to keep
this original arc and we want to make sure that we trim away and we blend to it.
So what I'm going to do is start a new sketch on the top plane,
and I want to bring that arc in as a reference.
So I'm going to select it and hit 'P' on the keyboard to project it and say "okay."
And then I want to hide my "landing gear" sketch.
So now, I can take my arcs,
and I can go from this point to the end and go from this point to the end as well.
Now, we want to select these two and make them tangent and as soon as we do that,
it automatically projects this edge in for us and do the same thing on the other side.
Make those tangent and now you can see that we've fully defined it.
Because these are not equal to each other,
we have a little bit different situation here.
We don't necessarily need them to be equal,
but we don't also have to add any more dimensions or constraints,
they're fully defined right now.
So at this point, we could use this as a trim for the surface,
but I also want to explore what this looks like when we thicken it.
So under "create," we're going to go down to "thicken" and we're going to select
this body and we want to thicken it inward eight millimeters.
Now, things get a little crazy when we do this because of the curvature in this corner.
But again, we're trimming that away,
so we're not too concerned with it.
So we're going to say "okay," and we're going to take a look at what we did.
So again, those corners,
those areas where the curvature change drastically.
The thicken doesn't look very nice,
but that's okay because again we're trimming it away and on the bottom,
you can see if we look at this from the front,
we don't have a nice flat area for us to land with.
Now if we show body three,
you can see here is the original body that we're working
with and what we'd like is a nice flat section where this goes to land.
If we go into our origin and we take a look at our planes,
you can see that this line right here,
which is our sketch,
intersects here and everything that's thickened is below it.
So that means that we can trim it away really without any problems.
We can get that nice flat geometry on the bottom.
But let's take a look at cutting this from the top.
So we have our sketch here and a couple of ways that we can do this is
to create an "extrude cut" like you normally would do with other geometry,
or we can come in to "modify" and say "split body."
So the body to split is going to be our thicken and are splitting tool,
we have to rotate around,
is going to be these edges.
Now it's only going to allow us to do one edge
because the one in between is not something that we sketched.
But that's okay we'll do one at a time.
So now, what it does is it creates two bodies from this one.
So you can see here "body eight" and "body seven".
If I hide "body seven," we'd take a look at it from the top,
the cut is nice and normal to our top plane,
which means if I rotate it around,
it's going to match this edge.
Even though it's thickened down in this direction right here,
it matches this edge.
So when we combine everything together,
we'll be perfectly fine.
So we're going to take a look at that sketch one more time.
We're going to use the same "split body,
" split this body,
we're going to use this sketch.
And, just another tip for you while I'm thinking about it,
if you hold down the left mouse button,
it will bring up a selection for you.
So we can instantly grab sketch curve without having to rotate around.
You can also change the way that you select by using
your selection priority and selection filters.
So right now, we have select through and you could simply
turn it to just select "sketch curves"
instead of "faces" and that would simplify the selection process as well.
So we're going to say "okay" and now body nine is the one we want
to keep and body eight is this corner that we don't need anymore.
In order to get rid of them in here,
we want to select them by holding down the "control key" or the "shift key,
" we want to right click,
and we want to select "remove."
If you select "delete," it will delete
those bodies as well as any relations that go with them,
that means any sketches,
any parent features, they will completely be removed.
But if you right click and you use the remove,
it actually puts a feature in the timeline,
that way you can go back and suppress or delete it
at any point in time to bring that feature back.
The next thing that we want to do is we want to trim away some material,
we want to round these corners as well.
So I'm going to go ahead, I'm going to hide "body top
copy" and I'm only going to keep "body three" and "body nine."
Now at some point in time, we will rename these bodies,
but as we go along and we create some of these features,
we want to make sure that until we get to the point where they're all combined in one,
we don't really worry too much about naming them.
So right now what I'd like to do is cut some more information away.
I don't think we need this brace here,
and I want to take away some material here,
to keep it as light as possible outside of the center of mass.
So we're going to achieve that by taking a look at the top down cut,
the sketch that's right here,
and we want to start a new sketch on the top plane.
So again, we're just going to grab the top plane and because we have these inside edges,
I'm going to go ahead and project those.
And I also want to project these two outside edges and say "okay."
I'm going to use an "offset."
I'm going to offset this in minus
10 millimeters and we'll do the same thing again using my marking menu.
The 12 o'clock position is going to be a "repeat" command.
So if I just hit the right mouse button,
you see "repeat offset" is in there,
and I'm going to repeat the offset on this bottom edge
here and notice that it doesn't allow me to select that bottom edge.
So sometimes, you'll get this when
an offset won't allow you to automatically select an edge,
but we can project it and then it will be available to use as an offset.
Notice that it's grabbing the entire chain now.
So if we turn off chain selection and reselect this edge,
it will just be a single entity.
So now, this one's not necessarily going to be 10 millimeters
because of the way that our curvature works out,
but we're going to come in minus 15 millimeters and see how that works out for us.
Now at this point in time,
the last thing that we need is to connect these edges to these right here.
So I'm going to do this by drawing a straight line and because we have tangency here,
that should automatically give us tangency there as well.
And now we have this inside profile that we can select to make our "extrude cut."
Now if you want to hide the body,
some time that can help as well and take a look at what we have.
So from a top view,
because we're using the "show profile" option,
you can see that these areas are able to be extruded,
but this area right here isn't.
And that's telling me that I don't have this line here,
and we need to project it.
So I'm going to use 'P' on the keyboard.
And now we have that complete close profile that we want to extrude cut.
You don't have to worry about trimming any of the excess off of here and honestly,
leaving it is a much better option because when you delete it or trim it,
it's going to remove this dimension.
So we're going to go ahead and leave that excess and stop the sketch.
We can hide the top down cut.
We can show "body three" and "body nine" and we can go back to
our model workspace and create an extrude and simply pull this up through.
Now under objects to cut,
if we expand this,
it will automatically cut "body three" in "body nine" for us and that's okay.
So this is the starting point of our landing gear.
And again, going back to the original way that we made this body by creating an extrude,
it simplifies the process of adding these additional bodies
because we know everything can be cut normal to the top plane.
We don't have to worry about the direction of curvature if
we're using a bunch of thickens or anything like that.
And another note for you, you could also create all this
as a single surface and then thicken it if you want it to.
The last thing that we want to do at this point in time is,
we want to get rid of this extra piece on the bottom.
So what we're going to do is create
a split body which we can do from the model workspace,
and our body to split again is this landing gear portion and the splitting tool
in our case is going to be the XZ or top plane, and we're going to say "okay."
So now if we take a look at this, "body nine,
" is this lower portion and if we hide it,
it gives us that nice flat bottom.
So I'm going to right click.
I'm going to remove "body nine" and now I've got the starting point for
our landing gear and our prop protection.
So again, it's good to save often.
I'm going to go ahead and make a new version of this.
"Save" and that way we can move onto the next step.
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