Designing a product is only part of the process. Now, can that product be manufactured? A CNC machinist works with computer numeric controlled (CNC) machines from generating the machine code to machine setup and run. Understanding both CAD and CAM is essential to this portion of a design. Even if you are not the end user who programs a machine, it is invaluable to know how it’s done. This knowledge translates directly to part design by helping make intelligent design decisions with manufacturing in mind. This course introduces you to the integrated CAD/CAM approach behind Fusion 360 CAD/CAM as well as 3D printed design setup and finally assembly and testing. All stages of product design in one place! After completing this course, you will be able to: • Explain the Fusion 360 integrated CAD/CAM manufacturing workflow. • Summarize the trends that are influencing the future of manufacturing. • Demonstrate knowledge and skills in foundational concepts of Fusion 360 CAD/CAM software. • Set up a Flight Controller. • Assemble a quadcopter. • Fly the final design.
Creating the base solid of a drone chassis
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En provenance du cours de Autodesk
Manufacturing Process with Autodesk Fusion 360
20 notes
À partir de la leçon
Waterjet Program
Most retail production quad and multirotor chassis are made of flat plates of carbon fiber or injection molded plastic. Flat plates of composite materials are often cut on a machine that uses high pressure water and abrasives. This allows you to cut almost any material without introducing heat, which could affect its structure and properties. In this week's lessons, we'll explore how to setup and validate a 2D waterjet cut on a quadcopter chassis.
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Autodesk Education
In this lesson, we'll be creating the base solid of a drone chassis.
After completing this lesson,
you'll be able to create a sketch slot,
use Mirror on a feature,
use sketch Circular Pattern, create a group,
rename a sketch, rename a feature, and use Extrude.
Let's carry on with the file from our previous example and edit our sketch.
At this point, we want to go into a sketch drop down and select "Mirror".
We're going to Mirror all the lines that are associated with this front right corner,
and we're going to Mirror
them about this horizontal construction that we created and say "Okay".
I'm going to use the right-click marking menu to repeat the Mirror.
We're going to now take all these lines,
we're going to select the circle as well,
and we're going to Mirror this about this vertical line,
and we're going to say "Okay".
So, notice now we have the basic layout of our quadcopter.
So this is going to allow us to create
some solid geometry and then we can create
another sketch that's going to allow us to remove material.
So, from here, let's stop the sketch.
You can press "Extrude" or you can hit "E" on your keyboard.
And we want to extrude all of this geometry out with the exception of
the four holes that we're going to use to mount the PDB as well as the flight controller.
And we're going to take this up five millimeters, and we're going to say "Okay".
We're not going to worry about applying fillets or adding
any additional geometry just yet until we start removing material.
Again, I'm going to go ahead and save this file.
That way, I'll always have this point to come back to.
I'm going to go back to a top view,
and I'm going to start a new sketch.
And again, I'm going to started on the top plane,
which is the XZ plane.
I want to show the frame base sketch because I want to use this location point to start
creating my mounting point or the holes that were going to use to create the motor mount.
I'm going to press "C" on the keyboard and draw a circle at
that center point with a 10 millimeter diameter and hit "Enter" twice.
Now I can hide the frame base shape sketch.
And now I can create the slots that we're going to use to mount the motors.
So, from the sketch, drop down,
select "Slot" and "Center to Center Slot",
and we're going to drop two slots.
Now, notice that we have again a lot of constraints.
I'm going to turn show constraints off for now,
and I'm going to move the slot a little bit out of the way.
This one automatically applied a vertical constraint,
but we're going to select the center construction line,
control select the center point of our 10 millimeter circle,
and we're going to place a coincident constraint.
Now, this means that the line can move up and down, it can extend,
we can change the diameter of the slot,
but it cannot move left and right because it's vertical and it has to hit this point.
Then, I'm going to hit "D" on the keyboard,
and I'm going to place a radius value of 1.5.
I'm going to go from this endpoint to the origin.
I'm going to give this a distance of seven.
I'm going to go from here to the origin and give this a distance of 12.
Next, I'm going to dimension this one with a radius value of 1.25 and hit "Escape",
select the center construction line,
controls select the center of our circle and make them coincident.
Because this one does not have a vertical or horizontal constraint,
it is free to move around.
We're going to go ahead and give it a distance from the origin.
This time we're going to say five millimeters,
which will allow us to cut all the way into that ten,
and then we're going to give it an additional distance of ten millimeters.
Hit "Escape", and notice that now we can drag it around,
it's still not fully defined.
We're going to hit "D" one more time,
and we're going to place an angle between these two of 45 degrees.
Once we have those two fully defined,
we're going to go to "Sketch",
"Circular Pattern", and we want to pattern both slots.
Now, with slots, we can double-click and automatically grab the tangency.
We'll select the center point,
and we'll change the quantity to four and say "Okay".
What this allows us to do is have four slots of
a three millimeter diameter for a larger motor,
and we have four slots of
two and a half millimeter diameter that will allow us to mount a smaller motor.
It gives us a little bit of flexibility in terms of
mounting a certain type of motor or a certain size of motor.
We're going to stop to sketch.
We're going to press "E" on the keyboard to extrude.
And notice that this is sketched on the top plane which is below the extrude.
So we can't instantly select it.
And there are a few ways that we can get around that.
We can simply rotate the model and select it from underneath,
we can hold down the left mouse button and select the profile this way,
or we can actually go into our selection priority and selection filters,
and we can turn off select all and select only sketch profiles.
So that way, we can select through solid geometry from the
top and grab only the sketch profiles as needed.
We're going to pull this arrow up.
Notice how it's automatically cutting through our solid.
We're going to change the distance to all,
and we're going to say "Okay".
So now we have that cut through.
We're going to go back to a top view,
go back to our selection filters,
and notice that there are a lot more selection filters inside of
the model workspace as opposed to inside of the extrude feature.
So, just note that this do change from time to time and
the selection filters can be very helpful depending on what type of work you're doing.
Let's go ahead and take this,
go to "Create", "Mirror".
And we're going to create a mirror based on features.
We're going to select the last extrude feature from the timeline,
we're going to select our mirror plane of the front plane,
and we're going to say "Okay".
We're going to use our right-click marking menu,
but we're going to do it quickly by holding down
the right mouse button and moving up at the same time.
We're going to select our extrude as well as our mirror feature.
And this time we're going to go across the right plane,
and we're going to say "Okay".
So now we have four extrudes.
And if we zoom in,
you'll notice that this is a very thin section here between this,
and we might want to make sure that we can adjust this.
So let's go back to our frame base sketch.
We're going to edit, and we're going to change the 30 millimeter diameter to 31.
And notice that all the tendencies update all the rest of the geometry updated fine.
We can now stop the sketch,
and now we have a little bit more room between the slots.
I'm going to rename sketch two to be motor mount,
and I'm also going to go down into my features.
And notice that I have extrude one and I have extrude two.
I'm going to right-click on extrude one and rename it to call it chassis base.
I'm going to right-click on extrude two and rename it to be motor mount,
and then we have the mirror features.
I'm going to take the mirror features,
as well as the motor mount,
hold down the "Shift" key to select them all.
And actually, I'm going to include the sketch in that as well.
I'm going to right-click and create a group.
We can also rename the group if we want.
And notice I named three different things motor mount.
We have a motor mount sketch,
motor mount group, as well as motor mount feature.
You'll notice that it allows us to keep that same name for all three of those,
and there's no conflict between any of them.
So this helps because we don't have to come up
with creative work around for naming some of
these features or sketches because the name is already used.
At this point, let's fit to screen,
go ahead and save our file.
So we can move onto the next step.
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