4.1.1: Phone Holder Guide

 Learning Objectives

• Review basic functionalities to create and utilize a sketch in Fusion 360
• Develop a phone holder sketch in Fusion 360

Step 0 - Familiarize Yourself with Your Workplace

1. Download Fusion 360

   • Download Fusion 360 [here].

   • The download is free for all students, but it requires verification.

   • It may take a few days to be verified as a student, so do not procrastinate.

2. Note

   Depending on your internet speed, it may take up to an hour to install Fusion.

3. ViewCube

   • In the top right corner is the View Cube.  (Figure 1)

   • This is the most convenient way to rotate around the part.

   • You can click on eachcorner orface tosnap to that view or drag the cube to rotate freely.

   • Hold middle click to drag your view around the part if using a mouse

4. Top Menus

   • At the top of the window, you will find your tools menus.

   • In this tutorial, we will primarily use the Solids (Figure 3) and Sketch (Figure 2) menus.

   • Below, you will find more information about the tools we willuse from these menus.

5. Timeline Navigation

   • At the bottom of the window is the timeline (Figure 4).

   • Use theselector tomove between steps.

   • You can also right-click on each step to edit, suppress, or delete them.

   • You will not need not need to navigate the timeline to model the part correctly, however if you make a mistake you can easily 

   • By clicking on the play button, Fusion will automatically create an animation of your part being built

6. Saving Your File

   • Before you start working, make sure to name your file and save it.

   • Fusion uses its own file management system.  When you save the file, it will be saved to the cloud and not your computer.

Caution

If you don’t save the file beforehand, Fusion will be unable to create a recovery file for you if you encounter issues.

Fig 1.) An empty workspace in Fusion 360

 

Fig 2.) The sketch menu allows users to sketch 2D shapes as references for 3D tools found in later steps

 

Fig 3.) The solids menu.  By using the solids menu, you can give 2D sketches volume.  
 

Fig 4.) Timeline In Fusion 360

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Step 1 - Create Sketch

1. In the Solids menu, select the sketch tool.

   • Locate the Sketch tool in the Solids menu.  (Figure 2, section 1)

   • Click on it to activate the tool.

2. Select a plane about the origin to sketch on.

   • Choose any face; this determines the orientation of the object when exported.

3. Sketch a rectangle

   • Using the Rectangle tool, sketch an 80 by 20 rectangle in the orientation shown below, with one point at the origin.

4. Dimension the sketch

   • Use the Dimension tool after you sketch the rectangle to ensure that all dimensions are accurate.  (Figure 2, section 1)

5. Confirm sketch

   • Click the green check mark when you are finished.

   • 

Fig 5.) A properly dimensioned side profile In Fusion 360

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Step 2 - Extrude Step 1

1. In the Solids menu, select the extrude tool.

   • locate the extrude tool in the solids menu (Figure 3, Section 1)

2. Select the sketch that you just created.

   • Click directly on the sketch in the workspace or from the browser on the left.

   • Ensure it is highlighted to confirm selection.

3. Type 50 to extrude the sketch 50 mm.

   • Enter the value in the input field that will appear when you select the extrude tool

     • You can also drag the arrow that appears when extruding to change the extrusion distance

   • Verify that the unit is set to millimeters.

     • Tip

       You can change the units in the input field to change the units of your extrusion.  The default workspace is in millimeters.

4. Check the 3D model to confirm the changes.

   • Refer to (Figure 6) for what the extrusion should look like during the modeling process.

   • Compare your model to the Figure to ensure accuracy.

5. Select OK when you are finished.

   • Click the OK button to finalize the extrusion process.  The ok button is located in the extrude menu which appears on the right.

Fig 6.) Extrusion step for the phone holder.

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Step 3 - Sketch Negative Space of Phone Holder

1. In the Solids menu, select the sketch tool.

   • Locate the Sketch tool in the Solids menu.

   • Click on it to activate the tool.

2. Select the 80x20 face of the extrusion (Figure 7)

3. Create the side profile sketch.

   • Create a line from the lower left corner to the top horizontal line with a 30 degree angle.

     • When you place the end of the line, ensure that an X appears on your cursor. This means that the line's end point coincides with the top horizontal line, and the contour is thus closed.

     • Continue to use the same line tool to make sure that all lines you are making stay connected

   • Create a connected horizontal line along the top of the rectangle, which is 5 millimeters long.

   • Create a line from the end point of this horizontal, which is 15 millimeters long, and is 30 degrees from the horizontal.

   • Create a perpendicular line from the end point of the last line, to the horizontal line of the rectangle.

   • Refer to Figure 7 for proper dimensions.

4. Confirm sketch

   • Click the green check mark when you are finished in the sketch menu at the top of your screen.

Fig 7.) Side view of the phone holder after the sketch is done

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Step 4 - Extrude Negative Space

1. Select the extrude tool

   • In the Solids menu, select the extrude tool.  (Figure 3, section 1)

   • Click on it to activate the tool.

2. Select the contours

   • Select the two triangular sections of the sketch you just created.

3. Extrude

   • At the bottom right of the menu, ensure the operation is set to Cut in the extrude menu to the right (Figure 8)

   • Drag the arrow through the entire model to complete the cut.

4. Select OK to finish the extrusion.

Fig  8.) mid extrusion process to remove sketch shapes spatially

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Step 5 - Sketch Back of Phone Holder

1. Select the sketch plane

   • Select the same face of the block as before.

2. Select the sketch tool.

3. Sketch positive geometry

   • Sketch a triangle on the back of the block to support the back of the phone.

   • Create a perpendicular line to the angled "back" which is 15 millimeters long

     • Refer to Figure 9 for the dimensions of the sketch.

   • Make sure the contour is closed, or else you won't be able to extrude in the following steps.

     • If your contour is closed, it will be highlighted when you hover over it after you confirm your sketch

4. Confirm sketch

   • Click the green check mark when you are finished.

Fig 9.)   A sketch for additional back support for the phone on the side profile of the phone holder

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Step 6 - Extrude the Back of the Phone Holder

1. Select the extrude tool.

   • In the Solids menu, select the extrude tool.  (Figure 3, section 1)

   • Click on it to activate the tool.

2. Select the sketch that you just created.

3. Set the extrusion length

   • Click on the opposite face of the sketch to make the extruded body extend to the other side.

   • Alternatively, you can manually input a distance of 50 mm.

4. Set the operation type

   • Ensure that the operation is set to Join, not New Body in the extrude menu on the right (Figure 8).

5. Select OK to finish the extrusion

Fig  10.)   An isometric view of the phone holder after the extrusion

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Step 7 - Sketch Attachment Point for Keychain

1. Select the sketch tool.

2. Select the bottom view of the part (80 x 50 face).

   • Refer to Figure 11 and Figure 12 for sketch placement.

3. Sketch the dimensions for an attachment point for a keychain.

   • Ensure that the attachment point has sufficient material on each side to prevent it from breaking off if it is too thin.

   • Sketch a rectangle the same width as the bottom of the part.  Make this rectangle 15 millimeters deep.

   • Sketch a circle in the middle of this rectangle.  Use the Sketch dimension tool to ensure this circle is in the middle of the rectangle. 

   • Use the sketch fillet tool (Figure 2 section 1) to round off the rectangle's corners with a radius of 5 millimeters.

     • Refer to Figure 11 for the dimensions of the sketch.

4. Click the green check mark when you are finished.

Fig  11.)  A properly dimensioned attachment point for a keychain.

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Step 8 - Extrude the Attachment Point

1. Select the extrude tool.

   • In the Solids menu, select the fillet tool.  (Figure 3, section 1)

   • Click on it to activate the tool.

2. Select the sketch that you just made.

3. Extrude the sketch 5 mm.

   • Ensure that the operation is set to Join.

4. Select OK to finish the extrusion.

Fig  12.)  An isometric view of the phone holder after the flange has been extruded.

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Step 9 - Fillets

1. Select the fillet tool.

   • Click on it to activate the tool.

2. Select the corners that you want to fillet.

3. Set parameters

   • Ensure that the tangency weight is set to 1, and that the fillet radius type is set to Constant and Rolling Ball.

4. Input a radius

   • To preview the fillets, input a radius.

   • Use a radius of 2 mm.

Fig  13.) A preview of 2mm fillets on the part.  The blue faces are selected so all corners on their edge are filleted.

Note

You can select the face of an object to fillet all attached corners

Caution

Fillets can greatly improve the functionality of a part by smoothing sharp corners, but they can also significantly increase the cost of machining a part. Always consider how the part will be manufactured when applying features like fillets.

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Step 10 - Check Your Work

Fusion 360 uses many menus, and it’s common for even experienced designers to miss features.

1. Check bodies

   • Check the Bodies tab in the top left to ensure that there is only one body.  (Figure 1, Section 1)

   • If there is more than one body, check if they are making contact.

   • If they aren’t making contact, review your sketches.

     • To edit past sketches, right click on them in the timeline and click edit.  This will show your past sketch and allow you to edit it.

2. Review sketches

   • Make sure that sketches are touching bodies where applicable

3. Check taper angle

   • Check the taper angle if your sketches are touching but your extrusion is not.

     • To check the taper angle, right click on the extrusion feature in the timeline and click edit.  This will show your past extrusion and allow you to edit it.

4. Join bodies

   • If the bodies are touching but not joined, select the Combine tool from the Solids menu and choose Join.  (Figure 3, Section 1)

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Step 11 - Create an engineering drawing

Engineering drawings are a standardized part across many different engineering disciplines. Their goal is to communicate and verify an entire design on a single sheet of paper. They are for communication and record keeping, and are a key way that engineers communicate.

Follow the instructions located [here] to create an engineering drawing of your design.

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Step 12 - Export Files as STL

1. Navigate to the paper icon in the top left and select the dropdown.

2. In the dropdown, select Export.

3. If you have not saved the file yet, it will prompt you to provide a name and choose a location to save the file in the Fusion library.

4. In the export menu, change the file type in the dropdown to STL.

5. This will allow you to 3D print this part.

Note

Many 3d printing softwares accept different file types including .OBJ, but it is most common to save files as STL due to how efficient they are.