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.
Generative design feature setup
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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.
Meet the Instructors
Autodesk Education
In this lesson, we're going to begin setting up our features for a generative design.
After completing this lesson,
you'll be able to: create an offset surface, project an edge,
offset sketch, create a surface trim,
create a sketch pattern,
and create a sketch mirror.
With the main structure of our body complete really left up to the engineer to
finish off the final mounding of the components and maybe some structural additions,
we're left with a bit more freedom on the design.
We want to talk a bit about generative design.
Now, Fusion 360 doesn't currently have the traditional generative design tape features.
And by this I mean, inputting some of the criteria of
your design and then getting an output of an organic shape that meets all that criteria.
Now, inside of simulation,
Fusion 360 does have something called shape generator that's currently in preview.
Now, that does allow you to add loads in C where the load paths are.
But we're talking a bit more organic here.
So what we want to do is we want to explore how to make
organic generative type features inside a Fusion 360.
In order to do that, we're going to be using these sculpt environment.
But we're going to get into some of the setup that
will make the sculpting a bit easier for us.
So the first thing that I want to do is I want to talk a bit
about where we're going to make this shape and what we're going to do.
Inside of these open pockets,
below them are going to be components such as the speed controllers,
the flight controller, and in various other components.
And these components generally get hot.
They produce heat as a byproduct of them using current.
So, we want to make sure that we keep enough air flow to them,
but we also want to add a bit more structure in this area.
So right now it's fairly open.
But by adding a bit of this generative type design,
we can increase the structure but still allow airflow.
So what we're going to do is we're going to be creating what's
called a pipe which is essentially
a subdivided shape that allows us to pick
a line or a path and it'll create a pipe for us.
And that allows us to push and pull vertices and blend it with other things.
So, the starting point for that is going to be offset surfaces.
So, to get started, we want to make sure that we have our component
active and that we navigate to the patch work-space.
Now, if you remember, we have body top,
body bottom, and the body top copy.
So, what we'd like to do at this point is we'd like to make a few offset surfaces.
So, we're going to take body top and we're going to go to create offset.
So we're going to take this and we're going to offset it down
into the main portion of our body.
Now, remember we have eight millimeters of thickness here.
So, we want to make sure that we split the difference.
We're going to have two layers of this generative type pipe that we're going to design.
So, we're going to come down two millimeters
and say "Okay" and then we're going to repeat
that command and we're going to offset this one minus four millimeters and say "Okay".
So now we can hide the top and then we have a top and bottom portion.
Now, at any point in time,
we can always double click on those in the timeline and let's say that we want
the bottom one to actually be a five millimeters so that it's a little bit closer.
We can go ahead and move that down a little bit.
So, as we're looking at this,
what we want to try to do is we want to try to set
up a sketch that's going to help us in that overall process.
So the first thing that I like to do or the first thing that I
want to do is I want to trim
these surfaces out so that I have an accurate location for where I want this to be,
where I want my features.
So, I'm going to start a new sketch.
The new sketch is going to be on the top plane.
So I'm going to start by hitting p on
the keyboard and I want to project this entire path here.
So I'm going to go ahead and go around and
project everything including the filleted corners.
And this means going over to the other side,
grabbing this fillet, and so on.
And the reason I'm doing this manually as opposed to trying to grab tangency around
these edges is because I want to make sure that I get the specific things I need.
And we don't have tangency across here,
we have sharp corners that we are still leaving sharp for now.
We'll probably take care of them in a little bit.
But right now, that helps us a little bit.
The next thing that I want to do is I want to offset that.
So, I'm going to take this and I'm going to offset it outward.
Now, if you remember, the thickness of the small wall here is two millimeters.
And I'm actually going to go out a little bit further.
I'm going to go out to minus five millimeters and say "Okay".
So now, if I temporarily hide the X star body, I have the original,
so I know exactly where the opening is and then I
have this extra piece out here where I can take
my sketch lines and what that would that will help me
do is that it will help me extend the geometry I'm working with,
and that way, I can come back into the model work space and I can split it and
cut it up and I can use combine or boundary fill to take care of the excess.
So, it's always a good idea to
make sure that we have a little bit of extra especially when we're dealing
with organic shapes that aren't necessarily going to
be perpendicular going into the walls that are surrounding them.
So, at this point, we're going to stop this sketch and
I'm going to mirror this body or rather the set of bodies.
So, from create, we're going to mirror both of
these offset bodies and we're going to mirror them across the right plane and say "Okay".
I'm also going to go ahead and I'm going to stitch them together.
I'm going to stitch the top two together and I'm going to stitch the bottom two together.
So that way they're one big surface.
And then next, I'm going to trim them.
And I want to trim them with the outside profile of
our sketch and I can trim both of them at the same time.
So, if we go to a top view,
I can select the areas that I want to trim.
Now, when you do this, you need to make sure that your trim tool is completely closed.
If it's not completely closed,
it won't allow you to select any of those regions.
So by selecting those two outside regions,
what I'm left with is body 18 and body 19 in
this case that give us an idea of where we're sitting at.
Now the reason I went across this specific design path is because this is not flat.
If it was simply flat, it would be a lot easier,
we could just create a plane and project it up.
But I want to keep this curvature.
Now, in our case, the curvature is very minimal.
But in some cases,
you might have rather extreme curvature.
So this process is going to help you figure that out.
The next step in the process is to figure out
where we want these pipes or these lines to go.
So I'm going to come down to my sketches,
I'm going to hide sketch 12 and we're going to start a new sketch.
Again, we're going to sketch on the top plane and I'm going to start
by drawing a line that goes from the center, straight down.
Any time you snap to geometry such as an edge on the surface,
it's going to project it automatically for you.
I then, I'm going to take a line,
and I'm just going to come down across that and hit escape.
Notice it automatically applied
perpendicular for me and that's good because I want to keep
that perpendicular relation because I also want lines to cross that are parallel.
So, what I'm going to do is I want to make this geometry.
Again, I'm going to extend it out because as we make a pattern of this go down,
this line right here essentially,
it's going to stay the same length but it's going to
get further and further away from that edge.
So, I'm going to start by going to
sketch a rectangular pattern and the object is going to be this,
and the direction is going to be along this line.
And then if I pull this out,
I can start to make copies of it.
I can increase the number of instances I have.
So, for instance, if we decide to do,
let's go all the way out to 70 and let's do seven.
So we have one every 10 millimeters.
That's going to be a pretty good. When I hit "Okay",
notice that these lines can now be extended because I didn't fully define them.
So that helps me because I now,
I'm able to make sure that they all extend past this shape.
Now, don't worry about the excess right now,
I'm not too concerned with leaving things under defined.
But I do want to come back and I want to place a dimension in here,
and I'm going to make this let's say seven millimeters from the edge.
That gives me probably about the same on this backside.
Now, at this point, we want to make sure that we have
the same type of geometry going the other direction.
And there are a few ways that we can handle this.
Let's start by doing a mirror.
So let's try to mirror all these lines.
And let's mirror them across this vertical line that we drew,
and it automatically makes the cross for us.
So now you can see that we're fully defined.
We have all these little sections here of all these various little lines.
Now, we're not completely done here because there are
some additional things that we need to consider.
But for right now, what we're going to do is we're going to
stop the sketch and we're going to save our file.
That way we can move on to the next step.
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