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.
Removing unwanted mass
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来自 Autodesk 的课程
3D Model Creation with Autodesk Fusion 360
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从本节课中
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.
与讲师见面
Autodesk Education
In this lesson, we'll talk about removing unwanted mass.
After completing the lesson,
you'll be able to link dimensions and create a sketch offset.
The last major thing that I want to do to
this body before we move on to creating some more geometry,
is to actually reduce the weight of it.
So right now, it's
just an eight millimeter thick section of 3D printed plastic and that's going to be fine,
but the additional plastic in certain areas isn't really adding much to the structure,
it's only adding mass.
So, what we want to do is we want to find a way that we can reduce that.
In order to do that, I'm going to create some sketches.
So first, I'm going to create a new sketch on
the top plane and I want to project this entire face.
So, I'm going to select the face,
I'm going hit P on the keyboard to project it.
Now, what this has done is it's brought that face in and it's
allowed me to grab all the internal and external edges.
So then, I want to create an offset.
And I will say that the projection stops at
this division where our landing gear is and that's
okay because I'm actually going to leave the landing gear solid,
because I do want it to flex and take some of
the loading but we're going make sure that we can
reduce some of the mass that's closer to the center of the quad copter.
So I have chain selection turned on and I'm going to take this entire outside profile.
Now, I want to bring it in two millimeters.
I want to do that again,
so I'm going to go hold on the right mouse button,
go straight up to repeat,
and I'm going to take this,
and I'm going to bring this one out,
and I'm going to have it two millimeters.
But right now, I'm going to leave it at 3.093.
So then I can double click on it and I can
click this two millimeter and link them together.
So as I go around, we're going to follow that same process,
we are going to offset this.
And again, I'll bring it out some amount.
I'm going to change that value to be d65 so that way,
I can change this one value and I can affect all the rest of them.
Carrying on down the line,
we're going to go here and if we just type in d65 into this box,
we can automatically use that value as well.
So we hit d65,
you will have to make sure that it's offsetting the correct direction though, d65.
Yours might not be d65,
so just keep that in mind that you want to figure out what
the original dimension is going to be for that two millimeter offset.
So now what we've done is we've created
this sketch where we've got this internal section that we can remove.
Now, before I actually remove anything I'm going to come in,
I want to hide this body so that I can look at just the sketch.
The reason this is important is because we need to think about some of these areas.
For instance, in this area,
we don't want to leave this small amount of material here,
we actually want to make sure that we connect to
this boss because we want to have enough structure for the motor.
So, I'm going to add some additional lines here.
And I'm going to bring those lines,
so this line has tangency there,
and I'm actually going to bring this line out perpendicular.
So we're going to be filling in that material there.
As we go to the other motor we're going to do the same thing,
I'm going to bring this line out.
It's going to have tangecy or be collinear.
And this one's going to come out perpendicular to this edge.
So that way when we are removing material,
we're leaving this section here connected to the boss of the motor,
so that way we have that additional structure there.
Other than that, all the other regions are going to be just fine.
So we can stop the sketch,
we can bring body 10 back and we can create an extrude cut.
So we're going to be selecting,
basically one selection we're going to select that one internal region.
But the differences is,
we have to decide the starting and ending points.
So instead of starting from the profile plane we're going to start from object
and I'm going to grab this top face and then we're going to go a distance.
Now, I'm going to tell it minus one and we're going to take a look at it.
So notice that it's not cutting anything here.
So, it says that it failed to project to surface.
So sometimes that does happen.
And remember, that instead of the top surface here we can
actually just select in this case we could select a surface,
an actual physical surface and we can project it up.
Now, if you get this error that says failed to project a surface,
it's a good idea to go to a top view and figure out if any of
your sketch entities are offset from the geometry.
Now, the problem that we're having here is because of
this cut right here is actually eating directly into that motor.
So this is telling me that I need to go back and I need to edit and adjust that sketch.
So go back in, we'll edit the sketch,
we'll hide the solid body temporarily and what we want to
do is we want to offset this circle two millimeters.
So, we're going to use an offset and we're going to offset
it two millimeters but we need to make sure that it's going the right direction.
So in our case, it's going to go out negative.
So we're going to say negative d65 and hit OK.
So you can see there,
that the extension that we did for the tangency and the
perpendicular doesn't have to go as far
but it is still needed and it will help that corner out.
Another thing that we can do is we can relocate that tangecy to be out further.
And the reason I say that is because,
in this case, with this edge,
we would actually have two corners to fill it and
that might produce some problems depending on the size of the fill that we want to add.
So I'm actually going to delete that so that we only have
this single corner here that we cannot fill it to.
Now, we're going to have to do the same thing to the other one. So we'll come down here.
We will create an offset of this that's going out minus d65 and then again,
we'll make sure that we don't have
any compound curves so we're going to get rid of this one.
So we just have this one individual edge that we need to add a fill it to.
So now, if we zoom back out we're going to bring body 10 back,
we'll rotate this around a little bit and we'll do another extrude.
So this time, the extrude is actually going to
be leaving a little bit more material around that motor.
So that's good because originally,
it was going to cut directly into it.
So now, if we start from object,
we'll start from here and we can cut a certain amount,
let's just say minus two and see what it looks like.
So now, we get a preview on the screen of what that looks like.
Now, if you remember, we have eight millimeters to play with here.
So I'm actually going to go down minus four and I'm going to say OK.
So we've cut that material out four millimeters.
I'm going to show that sketch again,
I'm going to do another extrude using
the same profile and this
time what we're going to do is we're going to start from the bottom.
So from object is going to be the bottom face and I'm going to cut up three millimeters.
So notice that it says failed to project.
And the reason it's failing to project in this case
is probably likely due to some geometry,
for instance this motor mount right here.
So it doesn't like the motor mount being cut because it exactly matches the edge.
So that does tend to produce problems sometimes.
If we say that we want to just go from the profile plane and we want to cut,
it's going to keep that square.
So in order to account for the motor on the bottom,
we need to make some adjustments here.
And one way that we can do that is we can adjust how much we're leaving around the motor.
On the topside, we're leaving two millimeters we're matching everything,
but we can actually redo this on the bottom side and leave
a little bit more so we don't have that issue.
I'm going to do this by modifying
the original sketch and I'm going to simply add another offset.
So I'm going to offset this edge one millimeter.
In this case, it's going to be minus one.
And sometimes, you might need to turn off that chain selection.
Now, it looks like it's producing some problems,
in order for us to do this we might have to go back to the original edge and this time,
we're going to offset it minus three and it takes that one, okay.
We'll do the same thing up here.
We'll take that original inside edge,
we'll offset it minus three.
Now, we have that additional edge.
So when we exit the sketch,
we want to make sure that we still are using the same profile on the top,
so we have two millimeter wall here.
But now, when we want to do and extrude from the bottom,
it's going to be taking it from that extra section here,
that extra millimeter that we added.
So now if we rotate this around we're going to start from object,
we'll select this bottom face and we'll extrude out,
we'll do three millimeters.
So now what it's done on the bottom is it's
left an extra wall here for a little bit of extra structure.
So it didn't like the fact that we were exactly matching this edge and that's okay,
it's okay for us to leave a little bit more structure on the bottom.
We can hide sketch 11,
fit to screen and take a look at what we've created.
So everything looks pretty good here obviously we need to
add some fillets and round these corners out.
But everything looks pretty good.
I'm going to go ahead and save my file.
So again, I have a point that I can always jump back to.
So that way we can move onto the next step.
