# Computer Aided Design Competition

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Please review the CAD Guide presentation that explains the fundamentals of CAD software prior to performing this lab. The presentation is listed underneath the title Lab 2 on the EG1004 Lab Manual.

# Objective

The objective of this lab is to use Autodesk Fusion 360 to modify a three-dimensional structure to increase its minimum safety factor while minimizing any increase in volume. The structures will be evaluated in competition using a competition equation that depends on the change in the structure’s safety factors and volumes.

# Overview

## Computer-Aided Design

Computer Aided Design (CAD) is the practice of using computer software to create, modify, or analyze models of three-dimensional products. Across engineering industries, CAD allows engineers to efficiently create dimensioned, scaled drawings that allow them to explore and refine ideas safely and cost effectively (Berselli et al., 2020). Autodesk 360, AutoCAD, Revit, Dassault Systèmes SolidWorks, and Sketchup Free are examples of CAD software. This exercise will use Autodesk Fusion 360 to explore the use of CAD to evaluate and improve the safety of a structure.

## Design Considerations

The safety of a structure is often defined by a metric called the safety factor (Musto, 2012). The safety factor is defined as the ratio of how much stronger a material is than the expected load. It is the measure of the load a material can sustain before permanent deformation or fracture. A common, acceptable safety factor is at least 3. Any value below that will likely lead to structural failure.

Every design decision made by an engineering team can impact the safety factor of a structure. This begins with the choice of material used for the project. The Young’s modulus, or modulus of elasticity, of a material is the measure of its tendency to deform when a force is applied in the axial direction. The yield strength of a material is the point at which the material begins to deform plastically, and the shape of the material is permanently altered. The Ultimate Tensile Strength (UTS) of a material is the maximum stress that the material can withstand before structurally failing, which usually involves bending permanently or breaking (Table 1).

Material Aluminum (Al) Steel Young's Modulus (GPa) Yield Strength (MPa) Ultimate Tensile Strength (MPa) 69 275 310 200 207 345 118 33 210 14 9 18

## Autodesk Fusion 360

In this lab, Autodesk Fusion 360 will be used to modify a part and evaluate its safety factor. Autodesk Fusion 360 is a cloud-based CAD software; it uses remote servers hosted via the Internet to process, store, compute, create, and analyze 3D models of structures.

The two workspaces in Fusion 360 that will be used in this experiment are Design and Simulation (Figure 1). The Design workspace creates mechanical designs that contain information about geometric constraints, and the Simulation workspace simulates applied loads on a design to observe the design's performance under those loads.

Figure 1: Fusion 360 Workspaces

There are two tabs in the Design workspace: Create and Modify. The Create and Modify tabs contain the functions needed for sketching and building a 3D model. They create and modify sketches when in Sketch mode (Figure 2).

Figure 2: Create and Modify Tabs in Sketch Mode

A Sketch creates the 2D shapes that are the bases for all 3D models. When first sketching the shapes, they do not have to have accurate dimensions or scale. Using the Sketch Dimension tool and the Constraints functions, the base shape and 3D model can be edited without starting over (Figure 3).

Figure 3: Before (Left) and After (Right) of Sketch Using the Sketch Dimension Tool

Once a sketch is complete, the Create and Modify tabs are also used to generate the 3D model (Figure 4).

Figure 4: Create and Modify Tabs in Model Mode

The Extrude, Sweep, and Loft tools are used to give direction and depth to the 3D model. Extrude projects the initial sketch outward to create a model. The Sweep tool creates a 3D model of a predetermined surface (profile) along a specific path. The Loft tool creates a 3D extrusion to connect two profiles of any shape (Figure 5). The Sweep and Loft tools are particularly useful for creating extrusions at an angle.

Figure 5: Examples of Extrude (Left), Sweep (Middle), and Loft (Right)

The Loft/Sweep Tutorial video demonstrates how to use these tools. Table 1 shows common Fusion 360 shortcuts.

Table 2: Common Fusion 360 Shortcuts
Command Windows Key Combination Mac Key Combination
Pan
Hold Middle Mouse Button
Hold Middle Mouse Button
Zoom
Roll Middle Mouse Button
Roll Middle Mouse Button
Orbit
Hold Shift + Middle Mouse Button
Hold Shift + Middle Button
Undo
Ctrl + Z
Command + Z
Redo
Ctrl + Y
Command + Z + Shift
Copy
Ctrl + C
Command + C
Paste
Ctrl + V
Command + V
Cut
Ctrl + X
Command + X
Extrude
E
E
Move
M
M

The Timeline function located at the bottom of the screen contains a record of the design history that can be modified or manipulated. The controls located to the left can be used to visit previous actions (Figure 6). The middle button will play the design history as an animation. The gray slider on the timeline can be dragged to different areas to show the design at a given stage. Actions can also be removed from the timeline and the design will automatically update itself if errors do not occur later in the timeline.

Figure 6: Timeline Function

The Simulation workspace can run simulations to test how a design will perform under real-world conditions. A Static Stress simulation, for example, analyzes the deformation, stress, and safety factor of a design from structural loads and constraints. The assumptions used in the simulationare based on a linear response to stress when the load being applied is known and constant. The results determine if a design will deform excessively or fail (break) from the loads applied. To run the tests, loads and constraints are placed on the design.

Constraints consist of fixed, pinned, and frictionless support options that prevent motion in specific directions. Fixed constraints prevent all motion and displacement of a part (Figure 7). This would mimic a screw holding a part in place. A pinned support prevents movement in radial, axial, and/or tangential directions, but allows a part to rotate. Frictionless constraints prevent movement normal to the surface. This mimics a wall or floor to prevent motion perpendicular to the surface.

Figure 7: Example of Fixed Constraints

A load is the force being applied to the design (Figure 8). The force is characterized by the direction, the point of application, and the magnitude of the force being applied.

A Mesh is a boundary along the design made up of polygons that determine the precision of the analysis test (Figure 9). The analysis is run at every vertex. More polygons in the mesh would deliver more precise results with longer simulation time. When a part is altered, it is essential to regenerate the mesh.

Figure 9: Example of a Mesh

• A lab PC
• Fusion 360

# Procedure

## Part 1. Setting up the File

1. Launch AutoDesk Fusion 360, click Create Account, and fill in the information. Important: Make sure to use an NYU email (Figure 10).
Figure 10: Fusion 360 New File Options

## Part 2. Learning Exercise

The following activity will be performed prior to the CAD competition to allow students to familiarize themselves with the software.

2. Change the workspace from Simulation to Design in the top-leftmost drop down. Set the units of the drawing to millimeters. The Units setting is found in the Browser on the left side of the window under Document Settings.
3. Select one of the inner faces and start a 2D Sketch by clicking Create Sketch (Figure 11).
Figure 11: Creating a 2D Sketch on a Face
4. Create a Center Diameter Circle with a diameter of 14 mm by clicking on the center of the existing circular cut. Click Finish Sketch (Figure 12).
Figure 12: Sketching a Circle
5. Go to Create → Extrude, which will be used to create a cylinder. Select both contours (Figure 13).
Figure 13: Creating a Cylinder
6. Change the Extent Type to To Object. Select the opposite inner face (Figure 14). Make sure the operation is set to Join.
Figure 14: Extruding Circle to Face
7. Select one of the base faces and begin another 2D Sketch. Select the 2-Point Rectangle from the Sketch section of the toolbar (Figure 15).
Figure 15: Point Rectangle
8. Draw a 10 mm x 6 mm rectangle starting by clicking once at one of the vertices of the flat border (Figure 16) to place one point of the rectangle and click one more time to place the second point of the rectangle. The lengths can be typed in before placing the second point of the rectangle (switching which value is changed is done using the Tab key). Press Finish Sketch.
Figure 16: Dimensions of Rectangle
9. Select the perpendicular face nearest to the rectangle (drawn in the previous step) and start a 2D Sketch. Draw a 10 mm x 4 mm rectangle 8 mm from the base. The horizontal side of the rectangle must be parallel to the previous sketch (Figure 17). To accurately measure the 8 mm from the base, select the Sketch Dimension tool. Then select the bottom horizontal edge of the rectangle and the edge shown in the purple image below, then move the cursor to the right, click, and the dimension should show up. Then edit the measurement to 8 mm.
Figure 17: Dimensions of Second Rectangle
10. Next, align the new rectangle with the one previously drawn. Use Constraints → Collinear, and select the left side of the new rectangle and the left side of the lower rectangle as shown in Figure 18. Then select Finish Sketch.
Figure 18: Collinear Constraints
11. Go to Create → Loft. Select the previous two rectangles as Profiles. Make sure to scroll down and change Operation to New Body, or Step 12 will not work properly. (Figure 19).
Figure 19: Lofting a New Body
12. Click on Construct → Midplane and select both of the inner walls (Figure 20).
Figure 20: Midplane
13. Go to Create → Mirror. Select the Loft as the Object and the Plane as the Mirror Plane (Figure 21).
Figure 21: Mirroring Steps
14. This part should look like Figure 22.
Figure 22: Mirrored Loft
15. Select the central base and start a 2D Sketch. Draw two 5 mm Center Diameter Circles with the origin on the center line 8 mm from the edge (Figure 23). Finish the Sketch.
Figure 23: Dimensions Circles
16. Start a 2D Sketch on the midplane. Click on Create → Arc → 3 Point Arc. Place the first and the second points in the centers of each of the circles created in the previous step, as shown in Figures 24-25.
Figure 24: Creating Arc
Figure 25: Creating Arc
17. Place the third point so that your arc looks somewhat similar to the figure below. You may need to adjust your view so it is oriented as shown in the figure below. Using Create → Sketch Dimension select one of the end points and the third arc point, drag the dimension straight up, as shown in Figure 26 and set it to be 9 mm. If the arc endpoints are shifted, use Constraint → Coincident on each arc endpoint and the center of their respective circles. Click Finish Sketch.
Figure 26: Creating Arc
18. Go to Create → Sweep. Select the two circles created in the previous step as Profiles and select the Arc as the Path. Go to Operation and choose New Body (Figure 27).
Figure 27: Creating Sweep
19. It should look like Figure 28. Save the design.
Figure 28: Finished Loft
20. Create a New Design and make a 2D Sketch by selecting any plane and create a rectangle 5 mm x 26 mm, as seen in Figure 29.
Figure 29: Rectangle Sketch
21. Extrude the rectangle by 1 mm (Figure 30).
Figure 30: Extruding Rectangle
22. A vector graphics file will be used in the DXF format provided by NYU. In the future, a logo can be designed using the Sketch tool. Download the Tandon Logo DXF File (this logo was converted from the file provided on NYU's identity page).
23. The downloaded ZIP folder must be extracted. Select Insert DXF under the Insert section of the toolbar (Figure 31).
Figure 31: Insert DXF Tool
24. The Insert DXF information dialog will appear on the right side of the window. For the Plane/Sketch, select the top surface (Figure 32).
Figure 32: Selected Top Surface
25. Click the folder icon next to the Select DXF file to upload the Tandon Logo DXF File. The logo should appear (figure 33).
Figure 33: Imported DXF Logo
26. Move the logo away from the origin by dragging it with your mouse (Figure 34). Alternatively, highlight the entire logo, and use the Modify → Move/Copy tool to move it.
Figure 34: Relocated DXF Logo
27. If the Tandon Logo imports incorrectly, as shown in Figure 35, follow Steps 28-29. Otherwise, skip to Step 30.
Figure 35: Incorrect Tandon Logo Orientation
28. Select the Modify → Move/Copy tool. For Move Object, select sketch objects. For Selection, click and drag to select the entire Tandon logo. For Move Type, select rotate. For Axis, select the top horizontal line and set the angle to 180°, as seen in Figure 36.
Figure 36: Flip About the Horizontal Line
29. Repeat Step 21, but for Axis, select the right vertical line and set the angle to be 180° (Figure 37).
Figure 37: Flip About the Vertical Line
30. The imported Tandon logo is shown in Figure 38.
Figure 38: Imported Tandon Logo
31. The vertical bar and Tandon School of Engineering portions of the logo are not needed. Select the bar and text to the right by clicking and dragging (Figure 39). Delete this portion with the Delete key on the keyboard (not Backspace).
Figure 39: Tandon to Delete
32. The logo must be scaled to fit the part. A base point must be selected to scale the sketch. The midpoint of the line on the right side of the box around the torch will be used as the base point, so a point must be placed there first.
33. Before placing a point, the sketch must be in editing mode. A sketch is in editing mode when the background turns into guidelines, and Finish Sketch appears at the top right of the window. Edit the logo by selecting Browser → Sketches and double-clicking on the tandon_logo_white sketch (Figure 40).
Figure 40: Sketches in Browser
34. Select the Create → Point tool. Place a point at the midpoint of the right side of the box around the torch (Figure 41). This is the base point.
Figure 41: Midpoint on Box
35. Right click the bottom left corner point of the box around the torch, When selected on the correct point, select Delete Coincident (Figure 42). You may also need to repeat this for the lines connected to the point.
Figure 42: Delete Coincident
36. Select the Modify → Sketch Scale tool. The Sketch Scale information dialog will appear on the right hand side of the window. For the Entities, circle the entire logo by clicking and dragging. Do not select the midpoint created in Step 34. If the midpoint was selected, clicking on the point again will unselect it.
37. Switch to Point and select the midpoint created in Step 34 (Figure 43).
Figure 43: Select Midpoint
38. In the Sketch Scale window, a third option will appear as Scale Factor. enter a scaling factor of 4.5 and click OK (Figure 44).
Figure 44: Scale Factor
39. Drag and re-locate the logo so it fits cohesive with the sizing. It should look like the logo in Figure 45.
Figure 45: Final Logo
40. Create a 2D sketch on one of the main faces where the logo was inserted. Go to Create → Text. Make the box smaller than the face, as shown in Figure 46. Type in the designer's name and format it so it is Bold and will be visible and cohesive with the size of the part. Some recommended setups are shown in Figure 46.
Figure 46: Text Tool
41. After writing, finish the sketch. It should look like Figure 47.
Figure 47: Recommended Dimension for Text
42. The design must be cut into the base. To do this, the Extrude tool will be used.
43. To cut the design, select Create → Extrude on the toolbar. The Extrude information dialog will appear on the right hand side of the window. Select the design profile, which is the area around the torch and each of the letters.
44. In the Extrude window, scroll down to Operation, and select Cut. Then set the Distance to -0.2 mm (Figure 48). Click OK. Save the design and return to the Bracket.
Figure 48: Engraved Part
45. The final model is shown in Figure 49.
Figure 49: Final Model
46. An assembly between the Plate and Bracket must be made. The Bracket file will be used. In this case, the engraved Plate will be the one floating, which means that it will be the one moving to arrange the pieces in the desired order. In the Bracket file, click on Show Data Panel in the top left corner, as shown in Figure 50.
Figure 50: Show Data Panel
47. Once opened, the preview of the Plate should be visible (Figure 51).
Figure 51: Preview
48. Click and drag the Plate from the left to the right, where the main screen with the part is. Drop the Plate here. It should look like Figure 52. Press OK.
Figure 52: Imported Plate
49. Both parts must be listed as components to create Arrangements between them. The Plate was imported as a component already, now the main part is the only one missing. To do this, right click on Bodies and select Create components from Bodies (Figure 53). This will create four different components.
Figure 53: Convert to Bodies
50. Click on Modify → Move/Copy and switch from Bodies to Components, as seen in Figure 54.
Figure 54: Option Selection
51. Select the midpoint of the Plate (Figure 55).
Figure 55: Selecting for Orientation
52. Modify the Plate so it matches the orientation on Figure 56 by clicking the round circles and rotating it. Press OK.
Figure 56: Orientation
53. The position of the Plate needs to be exact. Go to Modify → Align (Figure 57) and click the back of the engraved Plate and the lower wall of the part.
Figure 57: Align Feature
54. The order matters as it will move one part to the other. If the part is oriented incorrectly, click on Flip and then OK. It should look like Figure 58.
Figure 58: Correct Direction
55. Use the Align feature again and press the left border of the Plate and the inner border of the left wall of the part, as shown in Figure 59.
Figure 59: Border Alignment
56. Do the same with the bottom border of both parts, as shown in Figure 60.
Figure 60: Border Alignment
57. If the plate is oriented incorrectly, use the Flip option to re-orient the Plate.
58. At the end, it should look like Figure 61.
Figure 61: End Result

## Part 3. Fusion 360 Competition

This portion of the lab is a competition that requires teams to redesign an unsafe part to have a minimum safety factor. The competition rules are listed below. The winner of the competition will receive extra credit as detailed in the Grading Policy.

### Competition Rules

• The redesigned part must have a safety factor of at least 3
• The redesigned part must not have more than double the volume of the original part
• The applied forces and fixed constraints cannot be altered
• The thickness of the base and the proportions of the original part cannot be altered
• The supports can be altered if and only if they do not take away from or add to the base of the part
• Only aluminum, steel, copper, or lead may be used when modifying the part

• Equation (1), the competition equation, will be used in the competition. The volume will be measured in cubic millimeters.

(1)

### Design Consideration

• Do not simply add a long or large block to the redesigned part
• Consider bridges, cranes, and other systems that use structural support in the redesign
• Consider how material choices will impact the safety factor
• Consider how the part can be modified to support higher loads

### Parts Selection

There are seven parts to choose from for the competition (Figures 62 - 69). Click on the image of the part to download the Fusion 360 file for that part. Areas shown in red cannot be modified in any way. Components, such as fillets, chamfers, or other extrusions, including lofts and sweeps, can be added to the part.

### Procedure

1. Download the part to be modified as determined by the Lab TA. Extract the ZIP folder that was downloaded to obtain the F3D file.
2. Open Fusion 360. Go to File → Open and select the downloaded part. Select the Design workspace in the top left of the window (Figure 70).
Figure 70: Workspace Options
3. Open the Bodies in the Browser on the left hand side of the window, right click on the body of interest, and click Properties (Figure 71).
Figure 71: Properties of a Body
4. From the Properties dialog, record the volume of the body in cubic millimeters.
5. Click the workspace drop-down menu at the top left of the window and change the workspace to Simulation.
6. Open the Static Stress study in the Browser, and open the Study Materials tab (Figure 72). Record the material being used.
Figure 72: Study Material
7. Determine the location the load is being applied (Figure 73). Double click the blue force arrow and record the magnitude of the force in Newtons.
8. In the Browser, select Mesh (right click) → Generate Mesh (Figure 74). If the mesh is already generated and an error occurs, select OK.
Figure 74: Generate Mesh
9. In the Browser, right click Results and select Solve. Follow the Solve dialog until the simulation is complete. Click Close and the results should look like Figure 75.
Figure 75: Results of the Simulation
10. Record the safety factor for the design.
11. Sketch a possible solution that would add extra support against the force being applied, remembering what cannot be modified. Recall that the modified design must have a safety factor of at least 3. Have the sketch approved by a TA.
12. Go back to the Design workspace in Fusion 360 and use the tools shown to add support to the original part (i.e. Extrude and Sweep).
13. Once the part has been modified, go back to the Simulation workspace.
14. Change the material of the part, as it can increase the safety factor by right clicking on Study Materials in the Browser tab (Figure 76).
Figure 76: Study Materials
15. Click on the Study Materials (Figure 77) to open the drop down menu and change it to one of the four metals (Aluminum, steel, copper, lead).
Figure 77: Changing the Study Materials
16. Run the analysis again with the modified part by selecting Mesh → Generate Mesh in the Browser.
17. Solve the results and record the safety factor of the modified design. The design may become bent as the results are exaggerated in the simulation to gain a better understanding of how the part performs with an applied load.
18. If the safety factor of the modified parts is less than 3, add additional supports and/or change the material of the part and run the simulation again.
19. Once the required safety factor has been achieved, record the safety factor and volume of the modified part. Give the values of the safety factor and volume of the modified part to the TA to calculate the competition ranking.

# Assignment

## Individual Lab Report

Follow the lab report guidelines laid out in the EG1004 Writing Style Guide in the Technical Writing section of the manual. Use the outline below to write this report. Please only discuss Part 3, the Fusion 360 competition, in the lab report.

• Abstract
• Briefly summarize the lab exercise. Include the competition results
• Introduction
• Define safety factor and discuss the physical properties of materials observed in the lab
• Discuss Fusion 360
• Workspaces
• Tools and other components used in the lab exercise
• Discuss the competition
• Present the competition equation using Equation Editor and discuss it
• Discuss rules
• Discuss available materials
• Discuss design strategy and impact of rules, materials, and competition equation on design strategy
• Procedure
• Materials
• Describe what was done in sufficient detail so that another person could follow the description and replicate the results. Reference tools and workspaces used
• Data/Observations
• Present and discuss the first Fusion 360 simulation. Include simulation and all data
• Present and discuss all additional simulations. Include simulations and all data
• Present and discuss competition equation. Include the calculation using Equation Editor and initial and final safety factor and initial and final volume
• Present and discuss competition results. Include all data and table
• Conclusion
• Analyze competition results
• Discuss role of safety factor, volume, materials in determining competition results
• Discuss ways to improve the design’s performance in the competition
• Contribution statement

## Team PowerPoint Presentation

Follow the presentation guidelines laid out in the EG1004 Lab Presentation Format in the Technical Presentations section of the manual. When preparing the presentation, consider the following points.

• Why is CAD software, such as Fusion 360, AutoCAD, or SolidWorks, an important tool for engineers?
• Include the four basic CAD drawing views (top, most detailed side, front, and isometric) of the mechanical part before and after modifications (eight drawings total)
• How are simulations used in engineering design?
• Explain the material selected for the redesign of the part
• Define safety factor and discuss the physical properties of materials observed in the lab
• How did having a constrained volume impact the design process?
• How did the redesign compare with other redesigns?
• Did the material have an impact on the safety factor, and if so, why?

# Appendix

## Stable Mechanical Structure and Material Choice

A stable mechanical structure design will require a high safety factor. There are several methods to improve the design of a mechanical structure.

1. Effect of failure
1. Different types of design prefer different types of failure to lessen the risk of harm. Two types of failure include Brittle and Ductile failures.
2. Material of components
1. Materials are usually chosen based on different factors such as physical properties and mechanical properties. Physical properties are measurable for materials, such as density, melting point, conductivity or coefficient of expansion. Mechanical properties are how a material will react with different forces applied. Some examples consist of Young’s Modulus, yield strength and ultimate tensile strength.