4.2.1: Phone Holder Guide

Learning Objectives

• Review basic functionality to create an engineering drawing in solidworks 
• Develop a phone holder sketch in solidworks

Step 0 - Set up your workspace

1. Download Solidworks:

   • Access the student download for Solidworks [here]. (This download is free for all engineering students.)

• Tip

  Follow the instructions provided on the website to install the Solidworks Student Edition on your computer.

1. Create a Folder for Your Files:

   • In your E101 course folder, create a new folder named “Solidworks.”

Tip

This will help you keep all your Solidworks files organized.

1. Set the Unit System to Metric:

   • Open Solidworks, and in the bottom right corner of the screen, select MMGS to set your workspace to metric units.

   • Tip

     You might need to adjust this setting in future projects based on the unit system required.  Solidworks is in imperial units by default

2. Familiarize yourself with your workspace:

   • Below are screenshots of the two tabs you will be using: the features menu (Figure 1) and the sketch menu (Figure 2). Red boxes represent tools that you will use during this tutorial.

   • Tip

     All tools are located on the top by default, but the menu can be dragged to the side of the screen as well

Fig 1.) Tools available in the sketch menu

Fig 2.) Tools available in the features menu

Fig 3.) Tools available in the Sidebar.

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Step 1 - Create a New Part

1. Hover over the SolidWorks logo in the top-left corner.

2. Select File, then click New.

3. From the menu that appears (Figure 4), choose Drawing.

Fig 4.) Menu for selecting the type of document to create, including parts, assemblies, and drawings.

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Step 2- Selecting the work plane

1. Start a New Sketch:

   • Click on Sketch to begin creating a new sketch. (Figure 1, Section 1)

2. Select the Work Plane:

   • Choose the Front Plane from the available options (Fig 5, section 3).

Note

The front plane is typically the default print surface when exporting your design to an STL file

Fig 5.) SolidWorks display when hovering over a plane to select it

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Step 3- Sketching the Basic Contour

1. Start the Sketch:

   • Begin by sketching a rectangle with one point on the origin

   • Do not worry about dimensions, you will change that in step 3.2 and 3.3

2. Fully Define the Sketch:

   • Make sure all lines in your sketch are fully defined.

     • Add dimensions to every line to assign specific measurements using the smart dimension tool (Figure 1, Section 1).

       • To be fully defined means that all dimensions have only one associated measurement, not more or less.

     • If your sketch is fully defined, it will say "fully defined" in the bottom right corner next to where you changed your units.

   • Tips to defining a sketch

     • If any lines appear blue, the sketch is under defined and still moveable.

       • Test the sketch by attempting to move the blue lines. This will help you identify which dimensions are missing.

     • If your lines appear yellow, the sketch is over-defined.

       • Review your dimensions to ensure each line has only one defining dimension.

       • Remove any duplicate dimensions to correct this issue.

      

3. Review Your Work:

   • Ensure all lines are properly constrained and defined, with no remaining blue (underdefined) or yellow (overdefined) lines.

   • If all lines are black and all dimensions correct, press the blue arrow in the top right.

   • Note

     When you exit your sketch, the dimensions on your sketch will disappear.  They are still there.

      

Fig 6.) A properly dimensioned sketch for the profile of the phone holder

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Step 4 - Boss Extrude

1. Prepare for Extrusion:

   • Ensure that the sketch you just created is selected in the timeline (Figure 3 Section 1) on the left-hand side of your screen.

2. Select the Extrude Tool:

   • Navigate to the Features tab in the toolbar.  (Figure 2, Section 1)

   • Click on Extruded Boss/Base to start pulling your 2D sketch into a 3D object.

3. Set the Extrusion Depth:

   • In the Extrude settings, enter 50 millimeters as the extrusion depth. This will define how far your sketch is extended into the third dimension.

4. Review the Extrusion:

   • Before finalizing, make sure the extrusion preview looks correct.

   • Confirm that the extrusion is happening in the correct direction and that no other sketches are selected.

5. Complete the Extrusion:

   • Once you are satisfied with the settings, click the green check mark to finalize the extrusion, turning your sketch into a 3D object.

     • The green check mark can be pressed in the boss extrude menu on the screen's left or in the top right corner.

     • If you don't want to perform the extrusion you just made, press the red X in either the top right corner or the extrusion menu.

Fig 7.) A 50 mm extruded basic side profile.

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Step 5 - Select the Same Plane for the Second Sketch

1. Open the Sketch Tool:

   • click the Sketch tab in the top menu and click on the Sketch tool (Figure 1, Section 1) with a plane highlighted to start a new sketch on that plane.

2. Select the Same Plane:

   • Choose the same plane that you used for your initial sketch.

   • This ensures that your new sketch aligns with the previous one and maintains consistency in your design.

   • Verify that the selected plane is the same as before and is highlighted to indicate it is active for sketching.

3. Start the New Sketch:

   • With the correct plane selected, create your new sketch on this surface.

Fig 8.) An isometric view of the shape.  Orange lines around the face indicate that you are hovering over it and will be able to select it.

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Step 6 - Convert Entities

1. Open the Convert Entities Tool:

   • Go to the Sketch tab in the top menu.

   • Click on Convert Entities (Figure 1, Section 1).  This tool projects faces and closed geometry onto a selected sketch plane, making them part of the sketch. 

2. Select the Geometry to Project:

   • Choose the same view of the rectangle that you selected earlier. This action will project the contours of this face onto your current sketch plane.

   • The convert entities tool can project any closed face (such as the face of a cube) and any edge onto your sketch. However, open geometry (such as a sphere) cannot be converted.

3. Review the Projection:

   • Make sure to use the convert entities tab, which appears on the right, that you selected the correct faces.  The faces you are going to convert will appear highlighted

   • When you are happy with your selection, click the green check mark in either the top right and 

Note

You do not need to add dimensions to the projected lines made with the convert entities tool; they are projections of already constrained surfaces so they are already fully defined.

Fig 9.) Sketch after the application of convert entities.  

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Step 7 - Draw the Side Profile of the Phone Holder

1. Open the Line Tool:

   • Go to the Sketch tab in the top menu.

   • Select the Line tool (Figure 1 Section 1) from the options in the top left.

2. Sketch the Cutout:

   • Draw the outline for the cutout where the phone will sit. Ensure that this sketch matches the dimensions and location of the phone holder's cutout.

     • Start at one of the bottom corners, draw a line that extends to the top surface, and use the smart dimension tool to give it an angle of 30 degrees from the vertical.

       • If this line is not coincident with the line for the top surface, the contour will not be closed

     • Draw a line along the horizontal surface from the previous line's endpoint.  Use the smart dimension tool to make this line 5 millimeters long.

     • From the endpoint of the horizontal line, draw an angled line which is 20 millimeters long and at an angle of 30 degrees to the horizontal.

     • Draw a line which is both perpendicular to the previous line, and coincident with the horizontal top surface.

       • Use Relations to set both of these properties.

       • Relations can be set by selecting one or more lines with no other tool open, and selecting the desired relations from the sidebar.

   • Ensure that the lines you draw connect with the projections from Step 6. Align the new lines with the previously projected edges to ensure continuity.

3. Verify Relationships:

   • Look for green boxes at the ends of the lines. These indicate a relation between the lines (e.g., perpendicular, parallel, or coincident).

   • The image inside the green box will show the type of relation.

4. Review Constraints:

   • Ensure that all constraints are applied as required. This includes verifying that the sketch lines are properly constrained and aligned.

(An example of the constraints for Step 7 is shown below; notice the green boxes where the lines intersect with the sketch from Figure 9)

Fig 10.)  A view of the proper sketch constraints for the profile of the phone holder

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Step 8 - Extruded Cut

1. Exit the Sketch:

   • Close or exit out of the sketch you just created to return to the main workspace.

2. Open the Extruded Cut Tool:

   • Go to the Features tab in the top menu.

   • Click on Extruded Cut (Figure 2, Section 1) to start the cutting process. 

3. Select the Contours:

   • At the bottom of the  Feature Manager in the sidebar, select the two triangular contours you want to cut through.

     • You can also hover over closed contours with the Feature Manager open to select them.

4. Set the Cut Direction:

   • Under Direction 1, choose the Through All option. This setting will extrude the cut through the entire part without requiring a depth specification.  (Figure 11)

5. Review and Confirm:

   • Check the preview to ensure the cut is correct and will pass through the entire part.

   • Click the green check to finalize the extruded cut.

(An example of what the cut should look like is shown below.)

Fig 11.)  Extrusion process for the triangular surfaces

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Step 9 - Sketching the Back

1. Select the Same View:

   • Choose the same view that you used earlier in Step 5. This ensures that the new sketch aligns properly with the previous sketches.

2. Use the Convert Entities Tool:

   • Go to the Sketch tab in the top menu and click on Convert Entities to project the outline of the selected face onto the sketch plane.

3. Extend the Back Surface:

   • Draw an extension of the back surface by adding a new line parallel and concentric to the previous back with a length of 15 mm

     • You can ensure that the lines are parallel with either the relations or with the smart dimension tool

4. Close the geometry:

   • Add a line from the endpoint of the line you just drew to the end of the closed rectangular cross section

     • Make sure that the end points are coincident.  By doing this the lines will remain defined even if you chose to change the geometry later

5. Review Your Sketch:

   • Verify that the extension looks correct and that all dimensions are correctly applied.  (Figure 12)

Fig 12.)  A properly dimensioned back to the phone holder

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Step 10 - Extrude the Back

1. Select the Extrude Boss/Base Tool:

   • Go to the Features tab in the top menu and Click on Extruded Boss/Base (Figure 2, section 1) while keeping the sketch you just created selected.

2. Set the Extrusion Direction:

   • In the Extrude settings, under Direction 1, choose Through All to ensure the extrusion passes through the entire part.  (Figure 13)

   • If necessary, adjust the direction of the extrusion to ensure it extends properly from the back surface.

3. Review the Extrusion:

   • Check the preview to confirm that the extrusion extends correctly and aligns with your design.

4. Complete the Extrusion:

   • Once satisfied with the settings and preview, click the green check to finalize the extrusion.

Note

If the part cannot extrude, return to the previous step and check that all contours are closed. Open contours or gaps can prevent the extrusion from processing correctly.

Fig 13.)  An extruded back on the phone holder

 

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Step 11 - Keychain Mount

1. Select the Bottom View:

   • Choose the bottom view of the phone holder where you want to add the keychain mount.

2. Open a New Sketch:

   • Go to the Sketch tab in the top menu.

   • Click on Sketch to start a new sketch on the selected bottom view.

3. Use the Convert Entities Tool:

   • Click on Convert Entities to project the outline of the bottom face onto your new sketch.

   • This projection will help align the new features with the existing geometry.

4. Add the Keychain Hole:

   • Create a rectangle the length of the previous phone holder with a depth of 15 millimeters

   • Use the Sketch Fillet tool to round off the corners to a radius of 5 Millimeters

   • Draw a circle in the desired location on the bottom face. Ensure the circle is sized appropriately to fit a keychain.

     • Use the smart dimension tool to move the circle 25 millimeters from the side edge, and 7.5 millimeters from the back surface.  Give the circle a radius of 10 millimeters.

5. Extrude the New Feature:

   • Go to the Features tab in the top menu.

   • Click on Extruded Boss/Base.

   • Set the extrusion depth to 5 millimeters to add material around the hole, making the base of the holder suitable for mounting on a keychain.

     • Make sure that you are extruding the flange and not the circle.  You can select from different contours by hovering over them or by selecting them in the Feature Manager in the sidebar.

6. Review the Keychain Mount:

   • Check the preview to ensure the hole and extrusion are correctly positioned and sized.

(An example of what the keychain mount and dimensions should look like is shown below.)

Fig 14.) A properly dimensioned sketch of the keychain holder

Fig 15.)  A properly extruded sketch from Figure 14.

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Step 12 - Fillets

1. Open the Fillet Tool:

   • Go to the Features tab in the top menu and click on Fillet (Figure 2 section 1) to activate the tool that smooths out corners.

2. Set the Fillet Radius:

   • In the Fillet settings, set the radius to 2 millimeters. This will create a rounded edge with a 2 mm curve.

3. Select the Corners:

   • Click on all corners of the part where you want to apply the fillet, except for the bottom corners. Avoid the bottom corners to minimize overhangs during 3D printing, which helps in achieving a more stable print.

4. Review the Fillets:

   • Check the preview to ensure the fillets are applied correctly and the corners are smoothed as desired. (Figure 16)

Fig 16.)  A preview for a 2mm chamfer.

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 13 - 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 14 - Export as STL for 3D Printing

1. Prepare to Export the Model:

   • Once you're satisfied with your design, it's time to export it as an STL file for 3D printing.

2. Navigate to the Export Option:

   • Select File from the top menu.

   • From the dropdown menu, choose Print 3D.

3. Save the STL File:

   • In the menu on the left, scroll down and select Save to File.

   • Note that this menu is designed for sending files directly to networked printers, but most printers at NCSU do not use this method.

   • For non-networked printers, it's necessary to save the file locally on your computer.

4. Choose a Save Location:

   • Select where you want to save the STL file on your computer

Note

Other methods exist to export STL files in SolidWorks, but they are typically the fastest to open and slice.