Create a Fan Using Autodesk Fusion 360

This tutorial teaches you to build a part that you can actually use. It's based on this webinar that was recorded in June 2017. Although the parts we're creating are intermediate level parts, we're going to assume no prior Autodesk knowledge for this lesson. We'll be modelling an enclosure based on the DC hobby motor included in the Hackster box. The fan blade is an advanced part, so we won't be building it - we'll be simply adding it to our project afterward from the project files.

Measure the hobby motor

We'll be creating a 3D model of our hobby motor so that we can build an enclosure around it. That means you'll need to get measurements of the motor.

We've actually taken the measurements for you, so you if you don't have calipers but you do have the same hobby motor, you're in luck! We'll be basing the measurements in the rest of the lesson on these ones, so if you have a different hobby motor, be sure to note down the measurements and change them accordingly!

Install Fusion 360

Autodesk Fusion 360 is free for hobbyists, makers, and startups who makes less than $100,000 a year from using it. It runs on Mac and PC, and it's cloud-based, so you can sign in anywhere and work on your files. Download it here.

Quick overview of the tools in Fusion 360

In this project, we'll be using tools from the Sketch (creating new 2D geometry), Create (creating 3D geometry), Modify (change 3D geometry that you've already created), and Assemble (for putting all the parts together) toolbars. We'll also use Construction and Inspect, but won't explain them much.

The browser is the organized list of all the components in your project.

The sketch palette shows up on your canvas when you are working on a sketch. If you need to re-open it because you've stopped working on that sketch, simply right click on the component and select 'edit profile sketch' and the object will pop back into sketch view.

A mouse makes zooming and panning much easier. If you're using a mac, the trackpad works well, and you can find a handy list of shortcuts and trackpad gestures here.

Versioning in Fusion 360

In Fusion 360, each time you save, you get a new version which you can return to later if you mess up or want to go back. You can also see a timeline of all past commands at the bottom of the screen, so you can return to individual commands from each version.

Here are instructions for reverting to an older version.

Sketching the Hobby Motor

Open Autodesk to start a new design.

Click "Assemble" > "New Component" and name your new component "Toy Motor." Click "OK" and your component is created and shows up in the sidebar under the browser.

Now we'll start sketching the 2D geometry of our motor. Select "Sketch" > "Create Sketch" to start drawing your 2D geometry. When we create a sketch, we choose the 2 dimensional plane that we'll be drawing on from the 3D canvas. We'll be drawing on the front plane this time, so we can select it on the view cube, and then click it on the canvas to select it as the base for our 2D sketch. The sketch palette should pop up.

ANow we'll draw a rectangle that's approximately the size of the motor. Select "Sketch" > "Create rectangle" > "Center rectangle"

The software will ask you where you want to create your sketch. It doesn't matter that much where you create it. We'll align ours to the center by clicking on the center point. Click and drag until it looks approximately correct - don't worry about getting the dimensions exactly right just yet.

Select "Sketch" > "Arc" > "3-Point Arc". Place the first endpoint on the top of the rectangle you just drew and click the bottom of the rectangle to place the second endpoint. Click the third, middle endpoint in the middle.

We want the middle point of this arc to touch the edge of the rectangle. We've drawn it incorrectly on purpose. Now we can use constraints in the sketch palette to match it up perfectly with the edge of the rectangle.

With the arc still selected, choose the tangent constraint in the sketch palette.

Click the two things that you want to be tangent - the arc and the side of the rectangle. You'll see them squish together, placing the mid-point of the arc on the edge of the rectangle.

We also want the two sides of the arc to be aligned vertically, so choose the 'horizontal/vertical constraint' in the sketch palette. Then click the two points of the arc (they'll show a little dot when you hover over them). Now if you click and drag one point, the other one will follow since they're vertically aligned.

Let's create a line to bisect our rectangle by going to "Sketch" > "Line." You can easily find the horizontal midpoint of the rectangle because the cursor "snaps" to the midpoint (you'll see an x.) Draw a line through the middle of the rectangle, and then hit 'esc' to stop drawing lines.

Now we want to flip the arc shape over so we have two identical halves on either side of the midpoint. Do this by selecting "Sketch">"Mirror" and select the line you want to mirror (the arc) and the line you'd like to mirror it around (the midpoint) and click 'OK.'

We don't want the midline interfering with the rest of the geometry, since it was just used as a mirror, but we still want to keep it, so we can do that by turning it into a 'construction line' by selecting it and choosing "Construction" in the sketch palette.

Now it will just appear as a dotted orange line.

Now we're going to perfect our dimensions so that our fan is 20mm x 15 mm, which will perfectly fit our hobby motor (if you're using a different motor, obviously base it on that). Go to "Sketch" > "Sketch dimension" and select the top line. Type in '20' in the text box that appears.

Do the same for the vertical sides, but set them to 15mm. Finally, we want the arc edges to be 14 mm apart from each other on the horizontal side. Click the two mirrored arc points on the top and type in '14 mm'. If you drew your original geometry incorrectly or chose the wrong points, you may get a pop-up saying that your sketch is over-constrained. You can learn more about this error and how to fix it here.

You'll now see that all the lines on this sketch are black. That means that the sketch is fully defined, which means that you can no longer, for example, change the dimension of one side of the rectangle without throwing off the dimensions of the whole sketch. The sketch is now done! Choose 'STOP SKETCH' to tell the software that you're done with drawing in 2 dimensions, and ready to create a 3D object.

Extruding to create the 3D toy motor

The toy motor is about 27.5mm long, so we can simply do that using the 'extrude' command, which will squeeze our motor into being like spaghetti coming out of a spaghetti machine.

Choose "Create" > "Extrude". Select the object you'd like to extrude (the cylinder shape without the arc corners) and type in 27.5 mm.

Now we see a couple new objects in the browser. The object we just extruded has an origin, that lets us move it separate from the canvas, as well as a body which is the 3D representation of the sketch.

Now we're going to create the rest of the motor's odd angles by drawing and extruding a new sketch. We can actually sketch right on the surface of the 3D object.

Create a new sketch by clicking the "Create Sketch" button and selecting the back face of the model as the 2D geometry where we will be sketching.

Select "Sketch" > "Center diameter circle." Start drawing a center diameter circle on the end of your motor. You'll see the model shift to appear 2D again. Press "L" shortcut, and draw a line across your circle.

Then adjust the sizes of the shapes you just drew by selecting "Sketch Dimension" or using the "D" key shortcut. Click on the circle and make it 9.8mm. Click on the center and then click the line and make them 3mm apart.

Now choose 'Stop sketch', and choose 'Extrude' or click the "E" shortcut.

Select the area of the circle below the line, and the area around the circle. Click and drag inward (towards the opposite end of the motor), and you'll see the distance change to a negative measurement. -3mm should be perfect. Click 'OK'.

Now we're going to copy the steps above where we drew on the face of the motor. This time we're going to create a 2mm circle to extrude the motor shaft. Create a new sketch, draw a 2mm center diameter circle, stop sketch, and hit "E" for extrude. Extrude 2mm using the 'join' operation, which will fuse all of the separate 3D geometries together. Hit 'OK'.

Now one side is done, but we have to do the identical steps on the back. Click "Create Sketch" and draw a center diameter circle that is 6mm in diameter. Choose "Stop sketch." Extrude it 1.3mm.

Now we'll make our motor shaft on the back. The only differences are that we won't add the line across the circle and we'll make it 8mm long, as per our measurements. Once again, create a new sketch and use your center diameter circle tool to draw another circle inside the 6mm circle.

Now we're going to add a chamfer on the end of the shaft. Go to "Modify">"Chamfer" and select the end of the longer motor shaft.

Select 0.2mm to make a very slight chamfer and select 'OK'.

Now we'll use the 'Fillit' command to get rid of the sharp edges on the side. Select "Modify" > "Fillit", select all four edges of the motor (you won't have to rotate your shape probably, since this tool makes it easy to select just the edges) and give it a 2mm fillit, or whatever you think looks good.

Now save your project. It will prompt you for a 'location.' This is the project that the sketch is a member of, or basically just a shared folder.

Design the Enclosure

Select "Modify" > "Move/Copy". Select the motor and angle it to -20 on the X Angle.

We'll now start working on the enclosure. We need a new component for the enclosure, since it's a separate object from the motor. Go to "Create" > "New component." Name your new component "Housing." Where it says parent in the box, it should show that one parent component is selected. We want to make sure that this component is not a child of the toy motor component, since they're different parts and we may want to separate them out later.

Click the 'x' next to the currently selected parent, then select the top level part (should be "Desktop Fan vX" if you named your part "Desktop Fan") and hit 'OK'.

Your motor part will now appear transparent.

Create a new sketch. Fusion will start by asking you which pane you want to draw on. We don't want to draw on the component this time - we want to draw on the YZ plane of the canvas. It may be hard to select this with your mouse. To be sure to select the correct plane, click on the planes, and LEFT click and hold. A box will pop up and give us a choice of which plane or planar face we'd like to draw on. Select 'YZ."

Use the 'L' shortcut to start drawing with the line tool what your enclosure might look like. Use the parallel and perpendicular constraints in the sketch palette to make your enclosure look nice and fit around the motor.

Now we just need to dimension it, using the sketch dimension tool (D). You can select points, rather than lines, to get very precise dimensions on angled lines. You can also change angle dimensions by selecting lines that are at an angle or perpendicular to each other.

When you have the enclosure shape at a place that looks good to you, hit 'Stop sketch'.

Extrude the enclosure

Hit the 'E' shortcut to open the extrude tool. Rotate your shape using the view cube so you can see the width of the motor to get a good idea for how wide to extrude the fan enclosure. We want it to extrude in both directions, so choose 'Symmetric.' 15mm looks good to me, so I hit 'OK.'

Cut space for the motor out of the enclosure

We need to be able to cut out the front of the enclosure so that the motor can get through. Select the front face of the housing. Click 'Create sketch' to start a new sketch on the front face of the housing.

We'll be using the "project" tool. This tool projects geometry from outside of your sketch into your sketch. It works as if you were holding a flashlight up to your sketch and projecting its shadow onto whatever plane you're sketching on.

Hide the housing body by clicking the yellow lightbulb next to Body1 under the Housing component. The lightbulb should turn blue, and you'll be able to see the motor.

Select "Sketch" > "Project/Include" > "Project." Select the motor. Choose the body selection filter (the white one) since we want to project the entire body. Now if you hide the motor body (click the yellow light bulb again) you can still reference its outline. It's pink.

You can turn the housing's visibility back on.

Now we can start drawing lines to actually cut this out. First, we want one line that will represent the surface that the motor will sit on. Use the line tool to draw a line horizontally across the face of the housing, slightly off the bottom of the motor. Next, draw a line that goes through the middle of the object, but visibly off the actual middle. It's best to draw lines that are purposefully wrong so that we can easily apply constraints them using the sketch palette later.

Use the colinear constraint from the sketch palette to snap the bottom line into place with the base of the motor.

We'll use the coincident constraint to make sure it touches the middle.

We want to allow some wiggle room for our motor. Go to 'Sketch' > 'Offset'. Use the 'offset tool' to create a 0.2mm offset around the shape of the housing.

We also know that there are lead wires from the motor that stick out of the back, so we want to make sure there's room for them.

Using the line tool, make a line from to the top of the enclosure to the edge of the Fillit on the top right of the motor. Make a second line through the middle of the enclosure. Use the dimension tool to make the two lines 8mm apart.

Go to "Sketch" > "Mirror" and mirror the first line across the center line. Make the center line a construction line. Now use the line tool to draw a horizontal line at the top between the two mirrored points. Dimension it to be 2mm from the top of the enclosure. Choose 'Stop sketch.'

Select the Extrude tool. Select the motor shape on the enclosure, as well as the top piece we just drew. Be sure to select the offset as well, since it's not automatically selected. Don't select the bottom offset, since we'd like the motor to sit flat on the bottom surface.

We want to extrude it into the enclosure to be the same size as the motor. Hide the housing so that we can see the motor. In the 'extent' box in the extrude menu, choose 'To Object.' Select the back of the motor shaft as the distance we'd like to cut to. Under 'Chain faces' select the second option, 'Extend faces'. Choose 'Cut' rather than new body, since we want to cut this out of our current housing. Be sure to only choose the housing under 'Objects to cut.'

Design the shit out of it

This is looking pretty good! The one thing we're missing is space for the lead wires to come out the back. Also, it's a bit boxy. Let's get Deiter Rams on this thing!

Select "Modify" > "Draft." For the faces, select the two sides of the enclosure. For the plane, select the top, since we'll flare these two faces out from the top. There's a manipulator that let's you adjust and see what it would look like at different angles. We'll choose 5 degrees.

We'll draft the lower front face a bit as well. Select "Modify" > "Draft." Select the two side faces again. Select the bottom front as the plane. Select -5 degrees and hit 'OK.'

It looks slightly less boxy. Now we'll round the design a bit. Select "Modify">"Fillit" or press the 'F' shortcut. Select the four edges pictured. Give theme a radius of 1mm. Select "Modify">"Fillit" again and select the two side edges.

Now we'll separate the top and bottom of the housing, since we want the bottom part of the housing to be able to house our wires and battery.

Remember how we drew some lines on the housing in the last sketch? Turn the last enclosure sketch's visibility back on, so that we can use the lines we created there to split the body. Select "Modify" > "Split Body."

The "Body to Split" is the housing. The 'splitting tool' is the midline from the sketch. Select 'OK.'

Now our body is in two halves. Hide the bottom half so that we can see the top half clearly. We're going to split the top half into two pieces, since we want two pieces - one that the motor can rest on, and one hollow space behind it. Select "Modify" >"Split Body" again. Use the back of the motor shape as the splitting tool. The body to split is the entire top half. Select "OK."

We'll use the shell tool to hollow out the back part of the top half. Select "Modify" > "Shell". Select the back half of the body. Give it an inside thickness of 2mm.

Cut out room for the lead wires for the motor

We want to make sure that we have room for the lead wires, and that the motor has a place to sit. Select the bottom face of the most recently modified body. Create a new sketch. Select the bottom side of the toy motor as the plane you want to draw on. Choose the project tool from the Sketch menu and project the two parallel lines on the edge of the motor.

Choose the Line tool and draw a line perpendicular between the two parallel lines you just selected. Select the end of the two lines and use the Sketch Dimension tool ('D') to make the distance 10mm. Choose "Stop Sketch."

Now use the extrude tool to cut the shape out. Select the shape you just created and for the extent, choose 'To Object.' Cut to the bottom plane of the housing. Be sure to select just the housing to cut - deselect the toy motor.

Now we'll use the mirror tool to make the same cut on the other side of the top housing. This is the 3D mirror from the Create menu, so it's slightly different. Select "Create" > "Mirror." Choose the three faces that make up the feature you just cut as the objects. Choose the middle plane as as the mirror plane. Now the design is symmetrical.

Now we're done working on the top half, so we can combine the two halves back together by selecting "Modify" > "Combine."

Make space for the wires in the enclosure

Hide the top half and show just the bottom half. We again want to keep the front half of the enclosure solid so there is a place for the motor to rest, but hollow out the back half for wires and stuff. Again, choose "Modify" > "Split Body" and split the body from the end of the motor.

Choose "Modify" > "Shell" and choose the two faces, similar to the top half. Make it 2mm thick and click "OK."

Now the back is hollow, which is kind of a problem for keeping our tilted motor in place. We need to make a stopper to keep the motor from sliding too far back. Hide the back part of the housing so that you can clearly see where the motor would end.

Create a new sketch on the back part of the front half of the housing. Draw a center rectangle. Make it 5mm tall by 10mm wide (you can type in the height dimensions, then press 'tab' to enter the length dimensions). Click "Stop Sketch."

Use the Extrude tool to extrude the top of this rectangle 'To Object'. We'll extend this little rectangle to the back end of the motor. Hide the motor in the Browser to make sure we're not connecting it to the motor. Now we have a little stopper thingy in the back of the motor.

Now let's recombine the bottom part of the housing. Select "Modify" > "Combine" and select the two halves of the bottom of our housing. Click "OK." Now we just have two parts - a bottom half and a top half.

Add pins to keep the enclosure together

How will we keep the top half from sliding off the bottom half of our enclosure? Let's add some pins to the top half that will slot into holes on the bottom half.

Create a new sketch on the bottom of the top half of the housing. Draw a line bisecting one edge of the housing lengthwise. Using the symmetry constraint, select the two edges on either side of your line, as well as the line you just drew, so that it will snap two the symmetrical middle of these two lines.

Draw a 3mm center circle on your line. Use the dimension tool to position it 3mm from the front end of the housing. Turn the long line you just drew into a construction line. Hit 'Stop Sketch." Use the Extrude tool to extrude the pin 3mm.

Select "Modify" > " Chamfer" and add a 0.2mm chamfer to the end of the pin. This should help the pin to sit nicely in its slot. Now we'll mirror the pin to the other side. Select "Create" > "Mirror" and select the three faces of the pin (chamfer, top and body). Mirror it around the midplane.

Hide the top housing and show the bottom housing. We'll make some matching holes on the bottom housing. Create a new sketch on the top face of the bottom of the housing. Rather than guess where the pins are located, we'll simply project the pins from the top into the bottom half of the housing.

Select "Sketch" > "Project." Hide the bottom housing and show the top housing. Select the two pins and project them. Now we know where to draw our holes on the bottom half of the housing. We can turn them into construction lines by selecting them (use 'shift' to select multiple things at once) and hitting 'X.' Now simply use the center circle tool to draw some circles for the holes. Make them 3.1mm, to allow a tiny bit of space for our 3mm pins to get through. Hit 'Stop Sketch.'

Now we can extrude our holes into the bottom housing. We'll extrude them -2.2mm to allow a tiny bit of room for the housing to snap together.

We need to add a little hole for the wire to come out the back. Create a new sketch on the back of the bottom part of the enclosure. Draw a center diameter circle, starting at the midline. Use the dimension tool to make it 4mm diameter, and let the centerpoint sit 4.5 mm above the ground. Select 'Stop Sketch.' Extrude this circle 'To Object' and select the back of the motor as the object to extrude it to.

Final touches

We'll close off the top where we made room for the motor so it doesn't have a gaping hole.

Start a new sketch on this face. Choose "Sketch" > "Project/Include" and project in the motor. Use the 'Offset' tool to offset the projection by 0.2mm so that it matches the size of the hole in the enclosure. Choose "Stop Sketch." Use the Extrude tool to extrude the top piece we just created -10mm.

Add in the fan blade

Download the fan blade from here as a Fusion 360 archive: http://a360.co/2rVqVPE

Click "Upload" and you can now view the file in your Fusion 360 data panel. Right click on the fan blade in the data panel and select "Insert into current design." Select "Modify" > "Move/Copy" and move the fan slightly so that you can see it better.

If you make changes to the fan blade in this design, they'll be replicated in the original fan file.

We'll apply a joint to the fan blade. This is how parts are assembled in Fusion 360. The best way to think about this is which parts are not moving. Right click on the housing and choose "Ground." This will keep the housing from moving.

Select "Assemble" > "As-built Joint." This will join parts that are currently where you want them to be (as-built). Select the motor and the housing as the components. Click "OK." Now the motor and the housing are stuck together.

The joint command lets us join things that aren't currently in the correct location, like our fan blade. Select "Assemble" > "Join." We need to choose two components to align, in this case the end of the motor and the end of the hole inside of the fan. It might be difficult to select the end of the hole. On Mac, hold 'cmd'. On Windows, hold 'ctrl'. Now you can isolate the parts and select just the back. Choose "Revolute." This will allow the fan blade to spin. Hit "OK." If you click and drag on the fan, it can rotate!

The fan blade sticks out a bit too much. We can change the length of the shaft hole on the fan, either on our canvas or in the original file. In this case, it's probably easier to work on the original file, since we know the change we want to make and we don't have to hide the body of the housing and motor.

Choose "Modify" > "Press Pull." Move it -2.5mm further into the fan. Save it and make a note about what you changed, e.g. 'deepened fan's motor shaft hole.'

Now if you return to your original design and right click on the fan blade and choose 'get latest.' The fan blade should slide back closer to the housing.

Inspect and print your enclosure

Check your design by going to "Inspect" > "Section Analysis." This is useful for checking for overhangs and other flaws that will make 3D printing difficult. Choose the YZ axis so we split it down the middle. Looks pretty good.

Now go to "Inspect" > "Interference." Select all 4 bodies in our design and click "Compute." It tells us that no interference is detected. This means that no parts are in the way of other parts. Select "Include Coincident Form." This shows us the sides that are touching. The motor is resting on the place where it's meant to rest, and the top of the housing is resting on the bottom of the housing.

Good. Now we're ready to print. Select the housing body and choose "Save as STL."

That's it! Now just wire up your fan and you're ready to rumble!

Taylor Stein printed the fan and it actually does rumble because the motor has 0.1mm to shake, and it ends up being very noisy. It might be better to leave a slightly larger gap between that motor and the housing next time and fill it with a soft material like felt or a rubber gasket. Oh well, next time!