Difference between revisions of "Computer Aided Design (CAD) Competition"
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Latest revision as of 16:04, 13 May 2022
Please review the CAD Guide presentation that explains the fundamentals of CAD software prior to performing the lab. The presentation is listed underneath the title Lab 2 on the EG1003 Lab Manual.
The first experimental objective of this lab is to understand the fundamentals of computer aided design (CAD) software and 3D printing by designing an NYU logo keychain in Autodesk Fusion 360 and preparing it for 3D printing in Cura. The second objective is to modify a poorly-designed part using Autodesk Fusion 360 in a competition. The competition will be ranked by a design ratio that uses the part’s initial and final safety factor and initial and final volume.
CAD softwares, which include Autodesk's Fusion 360, AutoCAD, Revit, Dassault Systèmes SolidWorks, and Google SketchUp, allow engineers to make dimensioned, scaled drawings. These drawings are used to manufacture equipment, build infrastructure, and allow designers to display their designs with complete specifications and detail. Orthographic views (top, bottom, side, front, back) can be used to document the technical specifications in drawings needed for production while axonometric views (isometric, dimetric, trimetric) can be used to view the final 3D representation of a product.
This exercise will teach the basics of Autodesk Fusion 360, 3D file formats, 3D printing, and the skills needed to create simple 3D files and prepare them to be 3D printed.
Three-Dimensional Printing (3D Printing)
3D printing allows rapid prototyping and onsite manufacturing of products. Initially done with plastic, 3D printing now uses new techniques with new materials, such as aluminum, bronze, and glass. Biomaterials are also being used, such as 3D printing ear cartilage and liver tissue. As the 3D printing industry grows, 3D printing has become a significant part of many engineering fields.
In this course, 3D printing can be used to produce prototype components, building models, SLDP course modifications, robot parts, and a company logo.
Autodesk Fusion 360 is a cloud-based software that uses remote servers hosted via the internet to process, store, and compute data. This CAD tool creates precisely scaled drawings. These drawings are turned into 3D models that are used to visualize designs through photorealistic renderings and to simulate how a design performs under applied forces or loads. Fusion 360 can also be used for designing in computer-aided manufacturing (CAM), computer-aided engineering (CAE), animation, and more.
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 possibility of deformation or failure.
There are two tabs -- Create and Modify -- in the Design workspace. 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).
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).
Once a sketch is complete, the Create and Modify tabs are also used to generate the 3D model (Figure 4).
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.
The Loft/Sweep Tutorial video demonstrates how to use these tools. Table 1 shows common Fusion 360 shortcuts.
|Command||Windows Key Combination||Mac Key Combination|
The Simulation workspace can run simulations to test how a part will perform under real world conditions. A Static Stress simulation, for example, analyzes the deformation, stress, and safety factor in a model from structural loads and constraints. These assumptions are 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 model.
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 6). 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.
A Load is the force being applied to the model (Figure 7). 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 model made up of polygons that determine the precision of the analysis test (Figure 8). At every vertex, the analysis is run, and results are provided. The more polygons that are generated in the mesh, the more precise the results will be, but the longer it will take to run the simulation and produce the results. Always generate a new mesh when a part is altered.
Safety factor is 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, and any value below that is unacceptable and will likely lead to structural failure.
The physical properties of certain materials dictate how they behave under applied loads. The Young’s modulus, or modulus of elasticity, of a material is the measure of the stiffness of that material. It is described as the tendency of a material to deform axially 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 2).
Table 2: Allowed Materials and their Properties Material Aluminum Steel Copper Lead Modulus of Elasticity (GPa) 69 200 118 14 Yield Strength (MPa) 275 207 33 9 Ultimate Tensile Strength (MPa) 310 345 210 18
Materials and Equipment
- A lab PC
- Fusion 360
Part 1. Setting up the File
- Launch AutoDesk Fusion 360, click Create Account, and fill in the information. Important: Make sure to use an NYU email (Figure 9).
2. Designing the NYU Keychain
- Make the units of the drawing inches. They are in the Browser on the left side of the window under Document Settings.
- Start a 2D Sketch by clicking Create Sketch (Figure 10).
- Select the XZ plane (Figure 11).
- Select the 2-Point Rectangle from the Sketch section of the toolbar (Figure 12).
- Draw a 2.6 in × 0.7 in rectangle starting at the origin. Click once at the origin to place one point of the rectangle and click one more time to place the second point of the rectangle. The length values can be typed in before placing the second point of the rectangle (switching which value is changed is done using the Tab key).
- Select the Center Diameter Circle from the Sketch section of the toolbar.
- Draw a 0.7 in diameter circle centered in the middle of one of the 0.7 in sides of the rectangle (the cursor should become a blue X with a triangle and snap to the midpoint of the line) (Figure 13). Like the 2-Point Rectangle, the diameter of the circle can be user-defined.
- Draw another circle 0.45 in diameter in the same position. The sketch should look like Figure 14.
- Fillet (round) the corners of the base. Select the Fillet tool from the Modify section of the toolbar (Figure 15).
- Select one of the two intersecting lines that form the right angles on the base. Set the fillet radius to 0.125 in and repeat on the other corner. The sketch should look like Figure 16.
- Remove the extra lines using the trim tool. Select the Trim tool from the Modify section of the toolbar.
- Select all interior lines that divide the keychain to trim them. If error messages are indicated, remove the dimensions on the rest of the keychain by clicking on them and pressing the Delete key. The sketch should look like Figure 18.
- Exit the sketch using the Finish Sketch button in the top right of the window.
- After creating a 2D sketch, the next step is to use that sketch to create a 3D object. The Extrude tool will be used to create a 3D block. In the future, the Revolve or other tools can be used to create more advanced geometry. Select the Extrude tool from the Create section of the toolbar (Figure 19).
- The Extrude information dialog will pop-up on the right side of the window. Select the profile of the object to be extruded, which is the sketch that was just created. The sketch will highlight blue if it was made correctly. Click and change the Distance to 0.15 in and press the Enter key. Click OK in the Extrude information dialog. The model will look like the one shown in Figure 20.
- The next step is to add the design to the keychain. 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).
- The downloaded ZIP folder must first be extracted. Then, select Insert DXF under the Insert section of the toolbar (Figure 21).
- The Insert DXF information dialog will appear on the right side of the window. For the Plane/Sketch, select the top surface of the keychain (Figure 22).
- Click the folder icon next to the Select DXF file to upload the Tandon Logo DXF File. The logo should appear (Figure 23).
- Change the units to inches and click OK.
- 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 24). Delete this portion with the Delete key on the keyboard (not Backspace).
- The logo needs to be scaled to fit the keychain. A base point must be selected for which the sketch will be scaled to. 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.
- Before placing a point, the sketch must be in editing mode. A sketch is in editing mode when the background turns into gridlines, and Finish Sketch appears at the top right of the window. Edit the logo by selecting Browser → Sketches and double-clicking on tandon_long_white sketch (Figure 25).
- Select the Create → Point tool. Place a point at the midpoint of the right side of the box around the torch (Figure 26). This is the base point.
- Select the Modify → Sketch Scale tool. The Sketch Scale information dialog will appear on the righthand side of the window. For the Entities, circle the remaining lines of the box and torch of the logo by clicking and dragging. Do not select the base point in Step 24. If the midpoint was selected, clicking on the point again will unselect it.
- In the Sketch Scale window, a third option will appear as Scale Factor. Enter a scaling factor of 0.75 and click OK (Figure 27).
- The logo must now be positioned on the keychain. This will be done by drawing a line for alignment and moving the logo design to where the alignment line is located. Select the Sketch → Line tool and draw a 0.925 in horizontal line from a point close to the center of the hole in the keychain base to the right (Figure 28).
- Select the entire logo by clicking and dragging. Then select Modify → Move/Copy on the toolbar.
- The Move/Copy information dialog will appear on the right side of the window. The selection should already be made (the NYU logo). Select Point to Point as the Move Type. For the Origin Point, select the midpoint from the side of the box around the torch. For the Target Point, select the right end of the alignment line that was previously drawn (Figure 29). Click OK.
- Delete the alignment line that was drawn in Step 27.
- Click Finish Sketch in the top right of the window to exit the sketch. The final sketch is shown in Figure 30.
- To finish this side of the keychain, the design must be cut into the base. To do this, the Extrude tool will be used.
- To cut the design, select Create → Extrude on the toolbar. The Extrude information dialog will appear on the righthand side of the window. Select the design profile to cut, which is the area around the torch and each of the letters (Figure 31).
- In the Extrude window, scroll down to Operation, and select Cut. Set the Distance to -0.06 in (Figure 32). Click OK.
- The final model is shown in Figure 33.
Part 3. Fusion 360 Competition
- This portion of the lab is a competition to redesign a part and obtain the highest competition ratio
- 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
- The winning design will receive extra credit towards the lab report grade for this lab
- Only aluminum, steel, copper, or lead may be used when modifying the part
- Equation (1) will be used in the competition. (Please note the volume should be measured in mm3)
- 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 which material will increase the safety factor
- How can the part be modified to support higher loads?
Click on the image of the part to download the Fusion 360 file for that part. Figures 34 through 41 show the components that cannot be modified in red. The red areas cannot be cut, made longer, or thicker. Components, such as fillets, chamfers, or other extrusions, including lofts and sweeps, can be added.
- Download the part to be modified as determined by the Lab TA. Extract the ZIP folder that was downloaded to obtain the F3D file.
- Open Fusion 360. Go to File → Open and select the downloaded part. Select the Design workspace in the top left of the window.
- Open the Bodies in the Browser on the lefthand side of the window, right click on the body of interest, and click Properties (Figure 43).
- From the Properties dialog, record the volume of the body in mm3.
- Click the workspace drop-down menu at the top left of the window and change the workspace to Simulation.
- Open the Static Stress study in the Browser, and open the Study Materials tab (Figure 44). Record the material being used.
- Determine the location the load is being applied (Figure 45). Double click the blue force arrow and record the magnitude of the force in Newtons.
- In the Browser, select Mesh → Generate Mesh (Figure 46). If the mesh is already generated and an error occurs, select OK.
- 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 47.
- Record the safety factor for the design.
- Sketch a possible solution to the part 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.
- 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).
- Once the part has been modified, go back to the Simulation workspace.
- Change the material of the part, as it can increase the safety factor by right clicking on Study Materials in the Browser tab.
- Click on the Study Materials to open the drop down menu and change it to one of the four metals (Aluminum, steel, copper, lead.
- Run the analysis again with the modified part by selecting Mesh → Generate Mesh in the Browser.
- Solve the results and observe the safety factor of the modified design. The model may become bent as the results are exaggerated in the simulation to gain a better understanding of how the part moves with an applied load.
- 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.
- 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.
Individual Lab Report
Follow the lab report guidelines laid out in the EG1003 Writing Style Guide in the Technical Writing section of the manual. The following points should be addressed in the appropriate section of the lab report. Please only discuss the Fusion 360 competition portion in the lab report. The NYU logo keychain procedure does not need to be discussed.
- Briefly summarize the lab exercise. Include the competition results
- Discuss the uses and advantages and disadvantages of CAD software
- Discuss Fusion 360
- Tools and other components used in the lab exercise
- Discuss the competition
- Present and discuss ratio in Equation Editor
- Discuss rules
- Discuss available materials
- Discuss design strategy and impact of rules, materials, and ratio on design strategy
- For the competition, describe what was done in sufficient detail so that another person could follow the description and replicate the results. Reference tools and workspaces used
- Present and discuss first Fusion 360 simulation. Include simulation and all data
- Present and discuss all additional simulations. Include simulations and all data
- Present and discuss the Fusion 360 design’s ratio. 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
- 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
- Analyze competition results
- Contribution statement
Team PowerPoint Presentation
Follow the presentation guidelines laid out in the EG1003 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 is simulation used in engineering design?
- Explain the material selected for the redesign of the part
- How did having a constrained volume impact the design process?
- Define safety factor
- How did the redesign compare with other redesigns?
- Did the material have an impact on the safety factor, and if so, why?
Appendix: Preparing the Keychain for Print
This appendix entry is not a part of the lab, but serves as additional information to prepare the design in the 3D printing slicing software. The keychain made in the first exercise is used as a reference in this entry. Cura will be used for orienting parts on the printer build plate and selecting the color of each object. It also generates a code for the toolpath that the printer will read and follow to print the objects.
- Open Cura. If a menu pops up prompting for the printer, select the Ultimaker 3. If a menu does not pop up, make sure the printer currently selected is Ultimaker 3 at the top left corner.
- To load the two files from above, select File → Open File(s) at the top left of the window and open the STL files containing the base of the keychain and the keychain insert (Figure 50).
- In Cura, right click and drag to pan around, middle click and drag to move your frame of view, and scroll up and down to zoom in and out.
- Select the keychain base and click the Rotate tool from the toolbar on the lefthand side of the window. Use the red, blue, and green hoops to rotate the base so that the logo design is facing upward (Figure 51). Do the same for the keychain filler. Uncheck the Snap Rotation option for more precise rotation.
- Make sure both objects are lying flat on the build plate by using Rotate → Lay Flat. If the Lay Flat tool does not lay the object flat, go to the Move tool and type in 0 mm for the Z value (Figure 52.
- Select the rectangle insert, and using the Move tool on the left, enter 0.15 mm as the Z value to raise it vertically. If the insert does not move, go to Preferences >> Configure Cura and ensure the setting "automatically drop down to the build plate" is unchecked.
- Select the rectangle insert, and using the Move tool on the left, enter 0.15 mm as the Z value to raise it vertically. If the insert does not move, go to Preferences → Configure Cura and ensure the setting automatically drop down to the build plate is unchecked.
- Select the keychain insert and set it under Extruder 2 in the toolbar on the left (Figure 53). That piece will appear as slightly darker yellow. The insert must be set under a different extruder because it will be printed in a different color than the keychain base.
- Having the keychain insert selected, select the Move tool on the left-hand toolbar. Using the red and green arrows, drag the insert piece and align it in the keychain base (Figure 54). Make sure not to move the insert piece in the Z direction as this was previously set in Step 6.
- Click Slice, then click Save to File in the bottom right of the window. Save the file as a GCODE file.
No references being used in this lab.