Worldwide Sites

You have been detected as being from . Where applicable, you can see country-specific product information, offers, and pricing.

Thanks for your interest in Fusion 360, an email is on its way!

Looking to access a Fusion 360 project on your mobile device?

Get the Fusion 360 mobile app on:

Keyboard ALT + g to toggle grid overlay

## Simulate

Learn how to perform stress analysis to determine how loads lead to deformation and failure. This will help you understand if and how a part will fail.

### Overview

Get an overview of the types of simulations available in Fusion 360, and the things you need to consider.

• Simulation types

• Simulation considerations

• 2:25 min

• 1:18 min

### How to's

Select the right simulation type, learn some tips and best practices for setting things up, and be able to start an analysis from scratch.

• Static stress overview

• Structural buckling overview

• Modal frequencies overview

• Thermal overview

• Thermal stress overview

• Nonlinear static stress overview

• Event simulation overview

• Shape optimization overview

• 6:19 min

• 2:48 min

• 4:24 min

• 4:39 min

• 2:36 min

• 2:20 min

• 2:24 min

• 2:19 min

### Hands-on Exercises

Follow these step-by-step exercises to put your skills into practice, and establish the core skills you need to setup and solve simulations on your own.

• Static stress analysis of a connecting rod assembly

• Structural buckling analysis of a plastic table

• Adjust the length of a tuning fork to achieve the target pitch

• Thermal analysis of a radiator

• Thermal stress analysis of a disk break rotor

• Support beam with a non-linear material

• Event simulation of a snap fit assembly

• Lightweighting of a robot gripper arm

### Static Stress

x/x

#### Lesson: Static Stress Analysis of a Connecting Rod Assembly

In this tutorial we determine the effects of a 2,000 pound tensile load acting on a connecting rod assembly (consisting of the rod and two pins). Separation contact is defined between all contacting faces. They are free to slide along each other and separate but not penetrate each other.

We use two different method to analyze the assembly, as follows:

• Study 1: The model is constrained in the traditional manner (statically stable). The small pin is fixed at its end faces, and the load is applied to the end faces of the large pin. Additional constraints are added to prevent Y and Z motion of the connecting rod and large pin without inhibiting their deflection under load.
• Study 2: The model is completely unconstrained. Opposing (balanced) forces are applied to the end faces of the large and small pins. The Remove rigid body modes option is used to stabilize the model.

#### Open the Connecting Rod Assembly

In the Samples section of your Data Panel, browse to Basic Training > 11 – Simulation > Connecting Rod Assembly, as follows:

• If the Data Panel is not currently shown, click the Show Data Panel icon at the top of the screen. The Data Panel appears at the left side of the program window.
• The top level (home view) of the Data Panel is divided into two subsections: PROJECTS and SAMPLES. Scroll to the bottom of the PROJECTS list, if necessary, to see the SAMPLES list.
• Locate the Basic Training entry under SAMPLES and double-click it. The Data Panel now displays a list of the folders containing the training lesson models.
• Click the 11 - Simulation folder.
• Select the model, Connecting Rod Assembly.

#### Save the Model

When you open a sample model in Fusion for the first time, it appears in the MODEL Workspace. The model is read-only, and you must save a copy of it to a personal project.

1. Click File>Save As.
2. Optionally, create a Project to store your training models.
3. a) Click New Project.
b) Specify the project name.
c) Press Enter.

4. Optionally, create a folder within the project to store your training models.
5. a) Click New Folder.
b) Specify a folder name.
c) Press Enter.
d) Double-click the new folder to make it the current file saving location.

6. Click Save.

#### Access the SIMULATION Workspace

Select SIMULATION from the Change Workspace drop-down menu at the left end of the toolbar.

#### Choose the Units for the Simulation

You may have set different default units than are initially defined when Fusion 360 is installed. Also, the simulation units are independent from the units specified in the MODEL workspace. So, the units system can change when you switch to the SIMULATION workspace. Therefore, verify that the proper units are specified to be consistent with this tutorial.

1. Click the Edit icon that appears while the cursor is pointing at the Units node of the browser.
2. hoose U.S. (in) from the Default Unit Set drop-down list.
3. Click OK.

#### Create a Static Stress Study and Define its Parameters

1. In the SIMULATION toolbar, click New Simulation Study. Notice that none of the other simulation commands are available until after you create a study.
2. In the Studies dialog box, select Static Stress.
3. Click the arrow to the left of Settings to expand the settings frame of the dialog. The General settings appear initially.
4. Ensure that the Remove rigid body modes option is NOT activated. This option is applicable only to unconstrained models. In Study 1, we are including constraints.
5. Select Mesh from the left frame of the dialog to display the mesh settings.
6. Activate the Absolute Size radio button and type 0.1 in in the input field.
7. Click OK.

The rest of the SIMULATION workspace commands are now available.

#### Verify the Study Material

1. In the MATERIAL panel of the SIMULATION toolbar, click Study Materials, which is the default command in this panel.
2. In the APPLY MATERIALS dialog, verify that the values in the Study Material column are defined as follows:
• Connecting Rod: (Same as Model) or Aluminum 5052 H32. If not, select this material from the drop-down list.
• Large Pin and Small Pin: (Same as Model) or Steel AISI 1020 107 HR. If not, select this material from the drop-down list.
3. Click OK.

#### Constrain the Small Pin

1. In the CONSTRAINT panel of the SIMULATION toolbar, click Structural Constraints, which is the default command in this panel. The default Type of constraint is Fixed, and all three directions are constrained (Axis Ux, Uy, and Uz), which is what we want.
2. Click to select the top (+Y) end face of the small pin.
3. Click the bottommost corner of the ViewCube (the corner where the RIGHT, FRONT, and BOTTOM faces meet). This action produces a different isometric view of the model in which the underside is visible.
4. Note: The corner turns light-blue when the cursor is near to indicate the correct clicking zone for an isometric view.

5. Hold down the Ctrl key while clicking the bottom (-Y) end face of the small pin to select it too. The model look like the following image:
6. Click OK.

#### Constrain the Large Pin (Z-direction)

The cylindrical face of the large pin has been split to provide edges for applying constraints. Z constraints are needed at the straight edges to prevent the pin from rotating within the large hole. These edges lie in the XY symmetry plane of the connecting rod assembly. No displacement occurs in the direction normal to the symmetry plane (in this case, the Z direction). Therefore, we do not impede the natural deformation of this part under load by applying a Z constraint anywhere along an XY plane of symmetry.

There is a circular edge around the pin at the middle of its length. This edge lies in the XZ plane of symmetry. (The model, loads, and constraints are symmetrical about two planes: XY and XZ. Apply a Y constraint at this edge to prevent the pin from moving axially. Again, since this edge lies in a symmetry plane, a constraint in the normal direction does not impede the natural deflection of the part.

#### Constrain the Large Pin (Z-direction) … Continued

1. In the browser, expand the Model Components branch and then the Connecting Rod Assembly subbranch too.
2. Click the light bulb icon in the Connecting Rod:1 component heading to hide the connecting rod.
3. Right-click in the simulation canvas and choose Repeat Structural Constraints from the marking menu.
4. Next to Axis in the STRUCTURAL CONSTRAINTS dialog, deactivate Ux and Uy. We only want to constrain the Z direction this time.
5. Click both of the two visible straight edges on the large pin to select them. (Each edge runs half the length of the pin.) If you accidentally select a face, click again to deselect it.
6. Click the upper-left corner of the ViewCube as it is now oriented (the corner where the FRONT, LEFT, and TOP faces meet.
7. Click the remaining two visible straight edges on the large pin to select them too. The Target field of the dialog indicates that 4 Edges are selected, and your model should look like the image.
8. Click OK.

#### Constrain the Large Pin (Y-direction)

1. Right-click in the simulation canvas and choose Repeat Structural Constraints from the marking menu.
2. Next to Axis in the STRUCTURAL CONSTRAINTS dialog, deactivate Ux and Uz. We only want to constrain the Y direction this time.
3. Click both of the two half-circle edges located midlength of the large pin to select them. The Target field of the dialog indicates that 2 Edges are selected, and the model should look like the image.
4. Click OK.

Note: The large pin is constrained in the X direction only by virtue of contact with the connecting rod. In turn, the connecting rod is only constrained in the X direction by virtue of contact with the small pin, which is fully constrained. The connecting rod and large pin must be free to move in the X direction as the pins bend and the connecting rod stretches under load.

#### Constrain the Connecting Rod

To make the assembly statically stable, one more constraint is needed. Specifically, we must prevent rigid-body motion of the connecting rod in the Y direction. Again, constrain an edge along an XZ plane of symmetry, where no normal (Y) translation is expected.

1. In the browser, click the lightbulb icon in the Large Pin:1 component heading to hide the large pin.
2. Click the lightbulb icon in the Connecting Rod:1 component heading to show the connecting rod.
3. Right-click in the simulation canvas and choose Repeat Structural Constraints from the marking menu.
4. Next to Axis in the STRUCTURAL CONSTRAINTS dialog, deactivate Ux and Uz. We only want to constrain the Y direction this time.
5. Click the circular edge located middepth in the large hole of the connecting rod. The model should look like the image.
6. Click OK.

#### Apply the Force Load to the Large Pin

1. In the browser, click the lightbulb icon in the Large Pin:1 component heading to show the large pin.
2. In the LOAD panel of the SIMULATION toolbar, click Structural Loads, which is the default command in this panel. The default Type of load is Force, which is what we want.
3. In the STRUCTURAL LOADS dialog, set the Direction Type to Vectors (x, y, z).
4. Click the top (+Y) end face of the large pin to select it.
5. Click the bottommost corner of the ViewCube as it is now oriented (the corner where the FRONT, RIGHT, and BOTTOM faces meet.) This action results in a different isometric view, in which you can see the underside of the assembly.
6. Click the bottom (-Y) end face of the large pin to select it too.
7. Type -2000 in the Fx input field. Since we did not activate the Force per Entity option, the -2,000 pound force is divided among the selected faces. The areas of the two faces are equal, so each receives half of the total load (1,000 lbforce). Your model should resemble the image.
8. Click OK.

#### Automatically Detect Contact Sets

1. In the CONTACTS panel of the SIMULATION toolbar, click Automatic Contacts, which is the default command for this panel.
2. In the AUTOMATIC CONTACTS dialog, the default Contact Detection Tolerance for Solids is 0.004 in. Keep this value.
3. Click Generate. Contact sets are detected and the dialog closed.

#### Edit the Contact Type

Separation contact allows two bodies to slide along each other or freely separate from each other. However, the bodies cannot penetrate each other. This contact type represents the behavior of the actual connecting rod assembly our model represents.

1. At the Contacts node of the browser, click the Edit icon that appears when the cursor is over the heading. The CONTACTS MANAGER dialog appears.
2. Click the first row of the table to select it.
3. Holding down the Shift key, click the last row of the table. All table rows are now selected.
4. Using the drop-down list in any selected row of the Contact Type column, choose Separation. This contact type is applied to every contact set listed in the table. Keep the default penetration type (Symmetric).
5. Click OK.

#### Save the Model

The definition of contacts completes the simulation setup. Save the model before proceeding to the next page.

1. Click the Save icon at the top of the screen.
2. In the prompt that appears, type Study 1 Setup Complete in the Version Description field.
3. Click OK.

#### Run the Simulation on the Cloud or Locally

1. The Pre-check icon in the SOLVE panel of the SIMULATION toolbar is a gold exclamation point indicating that there is a warning.
2. Click Pre-check for details.
• Contact with the connecting rod controls the X displacement of the large pin.
• Contact with the small and large pins controls the Y displacement of the connecting rod.
• Contact with the small pin controls the X displacement of the connecting rod.
3. The warning indicates that the model contains one or more partially constrained groups. We expect this warning because the large pin has no X constraint applied, and the connecting rod has no X or Y constraint applied. We should not be concerned for the following reasons:

4. Click Close to dismiss the warnings.
5. Click Solve in the SOLVE panel of the SIMULATION toolbar.
6. Specify the computing location, using the radio button for solving On Cloud or Locally.
7. Note: Solving on the cloud consumes cloud credits.

8. Click Solve.
9. Note: This model may take several minutes to solve. The solution must be performed iteratively multiple times. The solver has to determine at what points along the contact faces the model is touching and where it is separating.

#### View the Total Displacement Results

When the solution is finished, the total displacement results are shown initially. Your displacement results should resemble the image:

#### View the Von Mises Stress

1. Using the Results drop-down list next to the plot legend, select Stress. The type of stress result initially displayed by default is the Von Mises stress.
2. In the SIMULATION toolbar, click INSPECT > Show Min/Max to show markers at the points of the minimum and maximum Von Mises stress results.
3. While holding down the Shift key, click the middle mouse button and drag the mouse to rotate the model viewpoint. Position the view so that you can clearly see the maximum and minimum stress points.
4. You can click and drag the Min and Max value balloons to a different position, as desired. Your stress results should resemble the image.

#### Restore the Default Result and Isometric View

1. In the SIMULATION toolbar, click INSPECT > Hide Min/Max.
2. Using the Results drop-down list next to the plot legend, select Displacement. Once again, the total displacement results are displayed.
3. Click the Home icon that appears above the ViewCube when the cursor is near. The display returns to the default isometric view of the model.

#### Clone the Study and Change the Settings

Make a duplicate of Study 1 but enable the Remove rigid body modes option for Study 2.

1. In the browser, right-click the Study 1 - Static Stress heading and choose Clone Study from the context menu. A Study 2 - Static Stress node appears in the browser, and the new study becomes the active one.
2. In the MANAGE panel of the SIMULATION toolbar, click Settings, which is the default command in this panel.
3. In the General section, activate the Remove rigid body modes checkbox.
4. Click OK.

#### Delete the Constraints

When you activate the Remove rigid body modes option, the solver applies a global acceleration load to produce a state of equilibrium. This global acceleration opposes and balances any imbalanced loads acting on the model (so that no constraints are needed). The model must either be fully unconstrained or constrained only in directions in which balanced loads (or no loads) are applied. In this exercise, we are only going to remove the fully fixed constraint that was previously applied to the ends of the small pin.

1. Expand the Load Case:1 branch of the browser in Study 2.
3. Right-click the Fixed1 heading under Constraints and choose Delete from the context menu.

Note: With this constraint removed, there is now no X constraint anywhere on the model. In the next step, we will balance the X loads applied to the model. Y and Z constraints remain, which is acceptable because no applied loads act in the Y or Z directions.

#### Add a Force to the Small Pin

1. In the LOAD panel of the SIMULATION toolbar, click Structural Loads. The default Type of load is Force, which is what we want.
2. In the STRUCTURAL LOADS dialog, set the Direction Type to Vectors (x, y, z).
3. Click the top (+Y) end face of the small pin to select it.
4. Click the bottommost corner of the ViewCube as it is now oriented (the corner where the FRONT, RIGHT, and BOTTOM faces meet.) This action results in a different isometric view, in which you can see the underside of the assembly.
5. Click the bottom (-Y) end face of the small pin to select it too.
6. Type 2000 in the Fx input field. Your model should resemble the image.
7. Click OK.

#### Restore the Default Isometric View

1. Click the Home icon that appears above the ViewCube when the cursor is near. The display returns to the default isometric view of the model.

#### Solve the Second Study

1. The Pre-check icon in the SOLVE panel of the SIMULATION toolbar is a gold exclamation point indicating that there is a warning.
2. Click Pre-check for details.
3. The warning indicates that no structural constraints are defined. We expect this warning because we are relying on the Remove rigid body modes option to stabilize the model instead of constraints.

4. Click Close to dismiss the warnings.
5. Click Solve in the SOLVE panel of the SIMULATION toolbar.
6. Specify the computing location, using the radio button for solving On Cloud or Locally. Notice that Study 1 is not selected because it has already been solved.
7. Note: Solving on the cloud consumes cloud credits.

8. Click Solve to run the simulation for Study 2, which is already selected.
9. Note: Again, this model may take several minutes to solve. The solution must be performed iteratively multiple times. The solver has to determine at what points along the contact faces the model is touching and where it is separating.

#### Access the COMPARE Workspace and Choose the Studies to Show

Perform the following steps after the solution has finished and the Study 2 displacement results have been displayed.

1. Select COMPARE from the Change Workspace drop-down menu at the left end of the toolbar. The toolbar changes to include commands specific to comparing results.
2. Two side-by-side contour plots appear. Typically, Study 1 appears in the left window, and Study 2 appears in the right window, which is what we want.
3. If necessary, use the drop-down menu in the lower-left corner of either window to select a different study to display.
4. Note: The results options, study selector, ViewCube, and Navigation Toolbar are only visible for the active window. Click anywhere within a Compare window to activate it.

5. Access the SYNCHRONIZE drop-down menu in the COMPARE toolbar and ensure that the following options are set:
• Synchronize Camera: Enabled
• Synchronize Result Type: Enabled
• Synchronize Min/Max: Disabled

#### Compare the Displacement Results

1. Click in the left window to activate it.
2. Using the drop-down menu near the plot legend, change the displacement type from Total to X. The X displacements appear in both windows, and your study results should resemble the following image:

Observations:

• Because one end of the Study 1 model is fixed, and the force stretches the assembly in the -X direction, all X displacement results are negative.
• For Study 1, the maximum relative X displacement magnitude for the assembly is about 0.0035 in.
• Since the Study 2 model is being acted on by +X and -X forces, positive and negative X displacement results are evident. The zero-displacement area is near the middle of the connecting rod span.
• The displacement variation for Study 2 is 0.00264 in to about - 0.00154 in. Therefore, the maximum relative displacement for the assembly is 0.0026 - (-0.00154 in), or approximately 0.0042 in.
• The deformation of the assembly is greater in Study 2, which is not surprising. The small pin is free to bend more without the fixed constraints on the end faces.

#### Compare the Stress Results

1. Using the drop-down menu near the plot legend, change the result type from Displacement to Stress. The Von Mises stresses appear in both windows, and your study results should resemble the following image:

#### Compare the Factor of Safety Results

1. Using the drop-down menu near the plot legend, change the result type from Stress to Safety Factor:

Observations:

• The maximum Von Mises stress for Study 1 is between 21,600 and 21,700 psi. The location, as we saw previously, is at the edge of the short pin. This pin behaves as a built-in beam, where the greatest moment occurs at the end supports.
• The maximum Von Mises stress for Study 2 is approximately 24,300 psi. It occurs on the surface of the small pin at its mid-length.

Tip: If desired, you can temporarily return to the SIMULATION workspace to hide parts and to show the Min/Max probes, which are not available in the COMPARE workspace. Do this to locate the maximum result when it is located on hidden faces.

• The Study 2 stress exceeds the Study 1 stress by approximately 12%.
• The safety factor results reflect the increased stress level in Study 2, where the safety factor is 25% lower than that of Study 1.

#### Compare the Contact Pressure Results

1. Using the drop-down menu near the plot legend, change the result type from Safety Factor to Contact Pressure:

Observations:

• The greater amount of small pin bending deflection in Study 2 results in a more localized contact area near the edges of the connecting rod hole. The end result is an 33% increase in contact pressure for Study 2, which is not surprising.

You have finished the Connecting Rod Static Stress Analysis tutorial.

### Structural Buckling

x/x

#### Lesson: Structural Buckling Analysis of a Plastic Table

Learn about Structural Buckling analyses. We set up and solve a Structural Buckling Analysis on a plastic table with two different materials. We investigate the results using several methods including the Compare Workspace.

In this tutorial, we learn the following key concepts:

• Navigate a model efficiently
• Apply Materials
• Apply Constraints
• Interpreting results
• Comparing thermal results between two studies on the same geometry

Note: Structural Buckling is only available in Fusion Ultimate.

#### Open the Plastic Table Model

In the Samples section of your Data Panel, browse to Basic Training > 11 – Simulation > Plastic Table, as follows:

1. If the Data Panel is not currently shown, click the Show Data Panel icon at the top of the screen. The Data Panel appears at the left side of the program window.
2. The top level (home view) of the Data Panel is divided into two subsections: PROJECTS and SAMPLES. Scroll to the bottom of the PROJECTS list, if necessary, to see the SAMPLES list.
3. Locate the Basic Training entry under SAMPLES and double-click it. The Data Panel now displays a list of the folders containing the training lesson models.
4. Click the 11 - Simulation folder.
5. Select the model, Plastic Table.

#### Save the Model

When you open a sample model in Fusion for the first time, it appears in the MODEL Workspace. The model is read-only, and you must save a copy of it to a personal project.

1. Click File > Save As.
2. Optionally, create a Project to store your training models.
3. a) Click New Project.
b) Specify the project name.
c) Press Enter.

4. Optionally, create a folder within the project to store your training models.
5. a) Click New Folder.
b) Specify a folder name.
c) Press Enter.
d) Double-click the new folder to make it the current file saving location.

6. Click Save.

#### Access the Simulation Workspace

1. Click the workspace selection in the top left corner.
2. Select the Simulation workspace from the drop-down list.
• Note: Notice that the toolbar changes to include commands specific to simulations.

#### Create New Structural Buckling Simulation Study

1. In the Simulation toolbar, click New Simulation Study. Notice that The New Simulation Study is the only available command at this point.
2. In the Studies dialog box, select Structural Buckling.
3. Click OK.

The rest of the simulation workspace commands are now available.

#### Apply Materials

1. Select Study Materials from the Materials section of the Workspace Toolbar.
2. Click Select All in the bottom-left corner to select all components.
3. Change the Study Materials for one of the drop-down menus to Plastic.
4. Click OK.

#### Constrain the Legs

We assume that the floor is rigid and slick for this tutorial. The legs can slide on the floor but are held in the Z direction. To keep the table from moving infinitely and allowing the analysis to solve, we lock the top surface from moving across the floor.

1. Click Constraints in the ribbon.
2. Click the Bottom face of the Navigation Cube.
3. Select the bottom face of all 4 legs of the table.
4. Ensure that the Type is set to Fixed and Targets states 4 faces.
5. Click Ux and Uy to deselect those axes. The legs can translate on the floor.
6. Click OK.

#### Constraints the Table Top

1. Click Constraints in the ribbon.
2. Click the Home icon near the Navigation Cube.
3. Select the table top.
4. Click Uz to deselect that axis. The model is now fully constrained even though no surface is fully fixed.
5. Click OK.

#### Apply a Force to the Table Top

We use assumptions or design criteria to determine Loads. We will check to see if the table could safely hold a 200 lb person.

1. Click Structural Loads in the ribbon.
2. Use the drop-down menu to ensure that the Type is set to Force.
3. Select the top of the table
4. Verify that the Vector arrows indicate that the force will compress the table.
5. Click Override Units and select lbforce.
6. Enter 200 for the Magnitude.
7. Click OK.

Tip: To easily find the buckling load without a force from design criteria use a value of 1 for the magnitude. The Buckling Load Factor is then the Critical Buckling Force.

#### Create Automatic Contacts

1. Click Automatic Contacts in the ribbon. Our parts are all coincident so the default tolerance is acceptable.
2. Click Generate.

#### Solve the Analysis

1. Click Solve in the Workspace Toolbar.
2. Specify On Cloud for the computing location. Structural Buckling Analyses do not allow local solve.
3. Note: Solving on the cloud consumes cloud credits.

4. Click Solve 1 Study.
5. Note: It will take several minutes for the analysis to mesh and solve.

#### Review the Buckling Modes

1. From the Buckling Mode drop-down list next to the plot legend, select Mode 1.
2. Click Animate in the RESULTS panel of the SIMULATION toolbar.
3. Activate the Two-way option to create a repeating sinusoidal animation that demonstrates the full buckling displacement as a cycle.
4. In the Speed drop-sown list, choose Fastest.
5. Click Play. Notice that not all the legs move in the same direction. The direction of the displacement in a buckling analysis is more qualitative than quantitative.
6. While the animation is still running, choose the next Buckling mode from the Buckling Mode drop-down list next to the plot legend. Observe the shape of this mode.
7. While the animation is still running, choose the final Buckling mode from the Buckling Mode drop-down list next to the plot legend.

#### Clone a Study

Notice that the first mode has the lowest buckling load factor. All three modes have a buckling load factor less than one, which means that buckling occurs. Typically the result you are looking for is the first positive load factor.

As with any design problem there is more than one solution to avoid buckling. In this tutorial, we clone the analysis and change the material to try to avoid buckling.

1. Right-click on Study 1 - Thermal in the browser. If a custom name was created right-click on the custom name.
2. Select Clone Study.

We now have a perfect copy of the settings from our previous study.

#### Modify the Materials

1. Select Study Materials from the Materials section of the Workspace Toolbar.
2. Click Select All in the bottom-left corner to select all components.
3. Change the Study Materials for one of the drop-down menus to PAEK Plastic.
4. Click OK.

#### Solve the Analysis

1. Click Solve in the Workspace Toolbar.
2. Specify On Cloud for the computing location. Structural Buckling Analyses do not allow local solve.
3. Note: Solving on the cloud consumes cloud credits.

4. Click Solve 1 Study.
5. Note: It will take several minutes for the analysis to mesh and solve.

#### Compare the Results

1. Click Compare in the Workspace Selection drop-down.
2. Note: The graphic window is now split, making two view windows. The displayed study is shown in the bottom left corner of each display window.
3. Click in the view window on the left to ensure it is active. When Active the display and navigation controls are at the bottom of the window in the center.
4. Use the Studies drop-down menu in the bottom left corner to select the first study.
5. Click in the view window on the right to ensure it is active. The display and navigation controls should appear along with the Studies drop-down menu.
6. Use the Studies drop-down menu in the bottom left corner to select the second study.

Note: Ensure that you are looking at the same Buckling Mode in both views, listed near the legend. If the Buckling Modes are not the same use the drop-down menu to change them in the active analysis.

#### Conclusion

We see that the shapes are the same and the displacement is also the same range with the different materials. The mode being the same is why the shape and displacement are the same. The buckling load factor is less than 1 in the first analysis, meaning that this buckling occurs with the given load. The second study has a buckling load factor greater than 1, so even though the shape and displacement are shown buckling would not occur.

We have successfully set up a buckling analysis, observed an undesired outcome and changed the design for improvement.

### Modal Frequencies

x/x

#### Lesson: Adjust the Length of a Tuning Fork to Achieve the Target Pitch

In this tutorial, we determine the frequency (musical pitch) of the first fundamental vibration mode of a tuning fork. We then adjust the length of the prongs and reanalyze the model to approximately achieve the desired target pitch.

• Design parameters:
• Tuning Fork Designation: A4 (440 Hz)
• Target Frequency: Approximately 95% of the desired musical pitch. 0.95 * 440 Hz = 418 Hz
• Note: The vibrating frequency increases as the prongs are shortened. The final pitch is precisely achieved by grinding material off of the ends of the prongs. Therefore, the prongs initially need to be slightly longer than the required length. This 5% grinding stock accounts for variations in manufacturing tolerances and material density and stiffness. It ensures that the rough cut fork vibrates at less than the standard A4 musical pitch. Therefore, material must be removed from the fork, and never has to be added to it, to achieve the final pitch.
• Material: Stainless Steel AISI 304
• No constraints applied: Because a tuning fork is held loosely in a person's hand, the model is unconstrained. Any fixed constraints would affect the resulting natural frequencies and mode shapes. Because the model is unconstrained, six rigid-body vibration modes are expected. We expect the seventh mode to be the one of interest.
• Mesh Size: Specify an absolute mesh size of 1.2 mm.
• Number of Modes to calculate: 12

#### Open the Tuning Fork Model

In the Samples section of your Data Panel, browse to Basic Training>11 – Tuning Fork – A4, as follows:

• If the Data Panel is not currently shown, click the Show Data Panel icon at the top of the screen. The Data Panel appears at the left side of the program window.
• The top level (home view) of the Data Panel is divided into two subsections: PROJECTS and SAMPLES. Scroll to the bottom of the PROJECTS list, if necessary, to see the SAMPLES list.
• Locate the Basic Training entry under SAMPLES and double-click it. The Data Panel now displays a list of the folders containing the training lesson models.
• Click the 11 - Simulation folder.
• Select the model, Tuning Fork – A4.

#### Save the Model

When you open a sample model in Fusion for the first time, it appears in the MODEL Workspace. The model is read-only, and you must save a copy of it to a personal project.

1. Click File>Save As.
2. Optionally, create a Project to store your training models.
3. a) Click New Project.
b) Specify the project name.
c) Press Enter.

4. Optionally, create a folder within the project to store your training models.
5. a) Click New Folder.
b) Specify a folder name.
c) Press Enter.
d) Double-click the new folder to make it the current file saving location.

6. Click Save.

#### Access the SIMULATION Workspace

Select SIMULATION from the Change Workspace drop-down menu at the left end of the toolbar.

#### Choose the Units for the Simulation

You may have set different default units than are initially defined when Fusion 360 is installed. Also, the simulation units are independent from the units specified in the MODEL workspace. So, the units system can change when you switch to the SIMULATION workspace. Therefore, verify that the proper units are specified to be consistent with this tutorial.

1. Click the Edit icon that appears while the cursor is pointing at the Units node of the browser.
2. Choose U.S. (in) from the Default Unit Set drop-down list.
3. Click OK.

#### Create a Modal Frequencies Study and Define its Parameters

1. In the SIMULATION toolbar, click New Simulation Study. Notice that none of the other simulation commands are available until after you create a study.
2. In the Studies dialog box, select Modal Frequencies.
3. Click the arrow to the left of Settings to expand the settings frame of the dialog. The General settings appear initially.
4. Type 12 in the input field below the activated Number of Modes checkbox.
5. Select Mesh from the left frame of the dialog to display the mesh settings.
6. Activate the Absolute Size radio button and type 1.2 mm in the input field.
7. Click OK.

The rest of the SIMULATION workspace commands are now available.

#### Verify the Study Material

1. In the MATERIAL panel of the SIMULATION toolbar, click Study Materials, which is the default command in this panel.
2. In the APPLY MATERIALS dialog, verify that the Study Material is (Same as Model) or Stainless Steel AISI 304. If not, select this material from the drop-down list.
3. Click OK.

#### Solve the Analysis

1. Click Solve in the SOLVE panel of the SIMULATION toolbar .
2. Note: Even though the model is unconstrained, the Pre-check icon is a green checkmark. This icon indicates that there are no warnings, and the model is ready to solve. The reason is that Modal Frequencies simulation models do not require constraints. The solver is able to output rigid-body vibrations as valid natural frequency modes.

3. Specify the computing location, using the radio button for solving On Cloud or Locally.
4. Note: Solving on the cloud consumes cloud credits.

5. Click Solve.

#### Display the Mesh

1. In the DISPLAY panel of the SIMULATION toolbar, click Model View. The mesh lines are easier to see on a light gray background than on the dark blue of the contour plot.
2. Click the light bulb icon in the Mesh node of the browser to turn on visibility of the mesh. Your model should look like the image:
• Note: The specified mesh size resulted in four elements through the thinnest portion of the tuning fork. This is a good element size for accurately capturing flexure of the prongs.
• Once again, click the light bulb icon in the Mesh node of the browser to turn off visibility of the mesh.
• In the SIMULATION toolbar, click DISPLAY > Results View, or press Ctrl-R.

#### Review the Other Mode Shapes and Frequencies

1. From the Mode drop-down list next to the plot legend, select Mode 1.
2. Click Animate in the RESULTS panel of the SIMULATION toolbar.
3. Activate the Two-way option to create a repeating sinusoidal animation that demonstrates the full vibration cycle.
4. In the Speed drop-sown list, choose Fastest.
5. Click Play. Notice that the tuning fork does not deform; it only translates in the X direction. The natural frequency for the rigid body modes in 0 Hz (or approximately 0 Hz).
6. While the animation is still running, choose the next vibration mode from the Mode drop-down list next to the plot legend. Observe the shape of this mode.
7. Repeat step 6 to view the next mode, until you have seen all twelve vibration modes. For each mode, observe the motion of the handle. Any mode that involves significant axial, radial, or torsional motion of the handle cannot be sustained. These modes will die out quickly when a person is holding the tuning fork.

#### Modal Shape Notes

Your Mode 12 results should look like the image:

Notice that the greatest displacement magnitude for Mode 12 is at the bottom of the handle, and it is in the +/- X direction. If someone is holding the tuning fork, this vibration mode will certainly die out almost immediately.

Note: Only modes 7 and 11 exhibit minimal motion of the handle. These two modes are the only two of the twelve calculated modes that can be sustained while someone is holding the tuning fork. Both of these modes involve a slight amount of axial motion (Y translation) at the handle. The relative axial motion is greater for mode 11. Therefore, it will die out faster than Mode 7 (the fundamental vibration mode).

#### Mode 7

1. From the Mode drop-down list next to the plot legend, select Mode 7.
2. In the ANIMATE dialog, click OK to stop the animation and close the dialog. Your model should look like the following image:

The natural frequency for Mode 7 is 471 Hz, which is about 7% higher than the nominal frequency of 440 Hz for the A4 musical note. Remember, that our goal is to produce a pitch or 418 HZ, which is 5% lower than the A4 note. We will have to lengthen the fork prongs to lower the natural frequency of this mode.

#### Access the MODEL Workspace

Select MODEL from the Change Workspace drop-down menu at the left end of the toolbar. Notice that the toolbar changes to include commands specific to modeling.

#### Lengthen the Prongs by 5 mm

1. Click the end face of one of the prongs to select it.
2. Hold down the Ctrl key and click the end face of the other prong to select it too.
3. Right-click in the modeling canvas and choose Press Pull from the Marking Menu. An arrow appears on the model, and a numeric input field appears in the model canvas. The arrow should be pointing outward. A positive distance lengthens the prongs, and a negative distance shortens them).
4. Type 5 mm in the numeric input field and press Enter.
5. In the INSPECT panel of the MODEL toolbar, click Measure.
6. Click the end face of one of the prongs. In the MEASURE dialog, Position Y should equal 75.00 mm. The centerline of the bend in the tuning fork is at Y=0. The original length of the prongs from the centerline of the bend was 70.00 mm. Since we added 5 mm to the length, 75.00 mm is the correct measurement.
7. In the MEASURE dialog, click Close.

1. Click the Save icon at the top of the screen to save the modified model.
2. In the prompt that appears, type 75 mm Prong Length in the Version Description field.
3. Click OK.

Select SIMULATION from the Change Workspace drop-down menu at the left end of the toolbar.

#### Solve the Model

1. Click Solve in the SOLVE panel of the SIMULATION toolbar.
2. Your computing location preference should have been retained from the original solution. Confirm that the appropriate radio button is still selected (On Cloud or Locally).
3. Click Solve.

#### Review Results of the Modified Model

From the Mode drop-down list next to the plot legend, select Mode 7. Your model should resemble the following image:

The frequency for this mode is 418 HZ, which is precisely the frequency we were targeting.

This lesson is completed. However, for an additional self-study challenge, proceed to the Last page of this tutorial in the help documentation.

### Thermal

x/x

#### Lesson: Thermal Analysis of a Radiator

In this tutorial, we learn about Thermal analyses. We set up and solve two different radiator designs. We also investigate the results using several methods.

• Navigate a model efficiently
• Interpreting results
• Comparing thermal results between two designs

In the Samples section of your Data Panel, browse to Basic Training > 11 – Simulation > Radiator, as follows:

1. If the Data Panel is not currently shown, click the Show Data Panel icon at the top of the screen. The Data Panel appears at the left side of the program window.
2. The top level (home view) of the Data Panel is divided into two subsections: PROJECTS and SAMPLES. Scroll to the bottom of the PROJECTS list, if necessary, to see the SAMPLES list.
3. Locate the Basic Training entry under SAMPLES and double-click it. The Data Panel now displays a list of the folders containing the training lesson models.
4. Click the 11 - Simulation folder.

#### Save the Model

When you open a sample model in Fusion for the first time, it appears in the MODEL Workspace. The model is read-only, and you must save a copy of it to a personal project.

1. Optionally, create a Project to store your training models.
2. a) Click New Project.
b) Specify the project name.
c) Press Enter.

3. Optionally, create a folder within the project to store your training models.
4. a) Click New Folder.
b) Specify a folder name.
c) Press Enter.
d) Double-click the new folder to make it the current file saving location.

5. Click Save.

#### Access the SIMULATION Workspace

Select SIMULATION from the Change Workspace drop-down menu at the left end of the toolbar.

#### Choose the Units for the Simulation

You may have set different default units than are initially defined when Fusion 360 is installed. Also, the simulation units are independent from the units specified in the MODEL workspace. So, the units system can change when you switch to the SIMULATION workspace. Therefore, verify that the proper units are specified to be consistent with this tutorial.

1. Click the Edit icon that appears while the cursor is pointing at the Units node of the browser.
2. Choose Metric (SI) from the Default Unit Set drop-down list.
3. Click OK.

#### Create New Thermal Simulation Study and Define its Parameters

1. In the Simulation toolbar, click New Simulation Study. Notice that The New Simulation Study is the only available command at this point.
2. In the Studies dialog box, select Thermal.
3. ck the arrow to the left of Settings to expand the settings frame of the dialog. The General settings appear initially.
4. Optionally, enter a different Name for the study.
5. Select Mesh from the left frame of the dialog to display the mesh settings.
6. Activate the Absolute Size radio button and type 10 mm in the input field.
7. Click OK.

The rest of the simulation workspace commands are now available.

Note: By using the Absolute mesh size we have ensured that our results are based on a comparable mesh size and are not modified based on the geometry.

#### Apply Materials

1. Select Study Materials from the Materials section of the Workspace Toolbar.
2. Click Select All in the bottom-left corner to select all components.
3. Change the Study Materials for one of the drop-down menus to Aluminum.
4. Click OK.

#### Suppress Unnecessary Bodies

1. Expand the Model Components section of the browser.
2. Right-click the Water node in the browser.
3. Select Suppress.
4. Note: Suppress removes the part from the mesh settings and the graphical window.

5. Click the checkbox next to the Fittings node on the browser. The browser appears the same for the Fittings as the Water. There is flexibility in the software allowing workflow personal preference.
• The model should appear similar to shown:

#### Select Inside Faces of the Pipe

1. Click the Lightbulb next to Fins in the browser to hide them.
2. Click the RIGHT face of the Navigation Cube.
3. Click Thermal Loads in the ribbon.
4. Use the drop-down menu to ensure that the Type is set to Applied Temperature.
5. Tip: The software will prevent you from putting incompatible loads on the same surface. Open the dialog and specify the load type before making a selection.

6. Click Select all faces to allow the selection of all the pipe surfaces.
7. Click the Pipe.
8. Click Select all faces to allow standard selection to be used to deselect the exterior faces of the pipe.
9. Left-click to the right and above the model and drag a window selection over the edges on the right side of the model.
10. Note: It is important to be pulling the selection window to the left to properly deselect surfaces.

Tip: Aligning the model using the ViewCube can make difficult selections much easier.

1. Click Override Units .
2. Select C from the drop-down list.
3. Enter 75 C in the Temperature Value input.
4. Note: The temperature would actually depend on the water heater or boiler. It is always a good idea to make a conservative assumption.

5. Click OK.

1. Click the Lightbulb next to Fins in the browser to show them.
2. Click the Lightbulb next to Pipe in the browser to hide it.
3. If the orientation was changed, click the RIGHT face of the Navigation Cube.
4. Click Thermal Loads in the Workspace Toolbar.
5. Change the Load Type to Radiation. Leave the default values for Emissivity 1 and Ambient Temperature Value 293.15 K (20 C).
6. Left-click and drag a window around all the Fins. 140 Faces are selected.
7. Click the arrow above the Navigation Cube.
8. Left-click to the left and above the top hole in the fins and drag a window selection over all the holes.
9. Note: It is important to be pulling the selection window to the right to properly deselect only the surfaces fully enclosed by the window. The previous window selection was to the left so that any surface touched would be selected (or in these cases deselected). There are now 84 Faces selected.

10. Click OK.

#### Apply Convection Load to the fins

1. Click Thermal Loads in the Workspace Toolbar.
2. Change the Load Type to Convection.
3. Left-click and drag a window around all the Fins. 140 Faces are selected.
4. Left-click to the left and above the top hole in the fins and drag a window selection over all the holes.
5. Note: It is important to be pulling the selection window to the right to properly deselect only the surfaces fully enclosed by the window. The previous window selection was to the left so that any surface touched would be selected (or in these cases deselected). There are now 84 Faces selected.

6. Enter 5 E-6 W/mm^2 for the Convection Value
7. Enter 293.15 K (20 C) for the Ambient Temperature Value. The ambient reference should be the same or the Loads will fight each other.
8. Click OK.

#### Create Automatic Contacts

1. Click Automatic Contacts in the Workspace Toolbar. Our parts are all coincident so the default tolerance is acceptable.
2. Click Generate.

#### Solve the Analysis

1. Click Solve in the Workspace Toolbar.
2. Specify the computing location, using the radio button for On Cloud or Locally.
3. Note: Solving on the cloud consumes cloud credits.

4. Click Solve.

#### Inspect Temperature Results

1. Right-click on the Model Components node of the browser and select Show all Components
2. Click the Home View on the ViewCube.
3. Temperature is the default result variable to be shown. If it is not, select Temperature from the result drop-down list near the legend.
4. Click INSPECT > Show Min/Max.

Note: The temperatures may vary slightly due to the mesh being coarse. The minimum Temperature is still over 70 degrees which can burn skin in under a second. We also see lines of high temperatures on the fins closest to the pipe.

#### Probe the High Temperatures

1. Click INSPECT > Surface Probe.
2. Click the model near the edge of the fins in the higher temperature regions in a few places. Compare the samples to validate they are not outliers (indicating a possible misplaced probe).
3. Click INSPECT > Hide All Probes

#### Inspect Heat Flux

1. Select Heat Flux from the result drop-down menu.

Note: Here we are looking at where the energy is able to move most efficiently. We notice that the highest heat flux is located where the model is expanding away from the hot pipes. The lowest temperature in the model were also in that same location.

Conclusions

The temperatures are too high throughout the model. The highest heat flux is near the ends of the fins where they extend furthest from the pipes. Increasing the surface area of the fins reduces the temperature of the model. The true power of simulation is that we can make a quick geometric change and understand its effects.

You have successfully completed a thermal analysis. Next we use the same settings on a model that has enlarged fins.

#### Open the Modified Model

In the Samples section of your Data Panel, browse to:

Basic Training > 11 - Simulation > Radiator Extended Fins

1. Click the Show Data Panel icon at the top of the screen, if the Data Panel is not currently shown. The Data Panel appears at the left side of the program window.
2. The top level (home view) of the Data Panel is divided into two subsections - PROJECTS and SAMPLES. Scroll to the bottom of the PROJECTS list if necessary to see the SAMPLES list.
3. Locate the Basic Training entry under SAMPLES and double-click it. The Data Panel now displays a list of the folders containing the training lesson models.
4. Click the 11 - Simulation folder.
5. Select the Radiator Extended Fins model.

#### Save the Model

When you open a sample model in Fusion for the first time, it appears in the MODEL Workspace. The model is read-only, and you must save a copy of it to a personal project.

1. Click File > Save As.
2. Navigate to the project and folder location that the first radiator model was saved.
3. Click Save.

#### Access the SIMULATION Workspace

Select SIMULATION from the Change Workspace drop-down menu at the left end of the toolbar.

#### Choose the Units for the Simulation

You may have set different default units than are initially defined when Fusion 360 is installed. Also, the simulation units are independent from the units specified in the MODEL workspace. So, the units system can change when you switch to the SIMULATION workspace. Therefore, verify that the proper units are specified to be consistent with this tutorial.

1. Click the Edit icon that appears while the cursor is pointing at the Units node of the browser.
2. Choose Metric (SI) from the Default Unit Set drop-down list.
3. Click OK.

#### Create New Thermal Simulation Study and Define its Parameters

1. In the Simulation toolbar, click New Simulation Study. Notice that The New Simulation Study is the only available command at this point.
2. In the Studies dialog box, select Thermal.
3. Click the arrow to the left of Settings to expand the settings frame of the dialog. The General settings appear initially.
4. Optionally, enter a different Name for the study.
5. Select Mesh from the left frame of the dialog to display the mesh settings.
6. Activate the Absolute Size radio button and type 10 mm in the input field.
7. Click OK.

The rest of the simulation workspace commands are now available.

Tip: Additional information can be modified through the settings if desired. More information can be found in the Settings page of the help.

Tip: The end goal of a simulation is to have results that are mesh independent. A typical workflow may include doing a mesh dependency study, changing the mesh to see the effect on the results. For this tutorial, we are using a relatively coarse mesh to reduce computing time.

#### Apply Materials

1. Select Study Materials from the Materials section of the Workspace Toolbar.
2. Click Select All in the bottom-left corner to select all components.
3. Change the Study Materials for one of the drop-down menus to Aluminum.
4. Click OK.

#### Suppress Unnecessary Bodies

1. Expand the Model Components section of the browser.
2. Right-click the Water node in the browser.
3. Select Suppress.
4. Note: Suppress removes the part from the mesh settings and the graphical window.

5. Click the checkbox next to the Fittings node on the browser. The browser appears the same for the Fittings as the Water. There is flexibility in the software allowing workflow personal preference.
• The model should appear similar to shown:

#### Select Inside Faces of the Pipe

1. Click the Lightbulb next to Fins in the browser to hide them.
2. Click the RIGHT face of the Navigation Cube.
3. Click Thermal Loads in the ribbon.
4. Use the drop-down menu to ensure that the Type is set to Applied Temperature.
5. Tip: The software will prevent you from putting incompatible loads on the same surface. Open the dialog and specify the load type before making a selection.

6. Click Select all faces to allow the selection of all the pipe surfaces.
7. Click the Pipe.
8. Click Select all faces to allow standard selection to be used to deselect the exterior faces of the pipe.
9. Left-click to the right and above the model and drag a window selection over the edges on the right side of the model.
10. Note: It is important to be pulling the selection window to the left to properly deselect surfaces.

Tip: Aligning the model using the ViewCube can make difficult selections much easier.

1. Click Override Units .
2. Select C from the drop-down list.
3. Enter 75 C in the Temperature Value input.
4. Note: The temperature would actually depend on the water heater or boiler. It is always a good idea to make a conservative assumption.

5. Click OK.

1. Click the Lightbulb next to Fins in the browser to show them.
2. Click the Lightbulb next to Pipe in the browser to hide it.
3. If the orientation was changed, click the RIGHT face of the Navigation Cube.
4. Click Thermal Loads in the Workspace Toolbar.
5. Change the Load Type to Radiation. Leave the default values for Emissivity 1 and Ambient Temperature Value 293.15 K (20 C).
6. Left-click and drag a window around all the Fins. 140 Faces are selected.
7. Click the arrow above the Navigation Cube.
8. Left-click to the left and above the top hole in the fins and drag a window selection over all the holes.
9. Note: It is important to be pulling the selection window to the right to properly deselect only the surfaces fully enclosed by the window. The previous window selection was to the left so that any surface touched would be selected (or in these cases deselected). There are now 84 Faces selected.

10. Click OK.

#### Apply Convection Load to the fins

1. Click Thermal Loads in the Workspace Toolbar.
2. Change the Load Type to Convection.
3. Left-click and drag a window around all the Fins. 140 Faces are selected.
4. Left-click to the left and above the top hole in the fins and drag a window selection over all the holes.
5. Note: It is important to be pulling the selection window to the right to properly deselect only the surfaces fully enclosed by the window. The previous window selection was to the left so that any surface touched would be selected (or in these cases deselected). There are now 84 Faces selected.

6. Enter 5 E-6 W/mm^2 for the Convection Value
7. Enter 293.15 K (20 C) for the Ambient Temperature Value. The ambient reference should be the same or the Loads will fight each other.
8. Click OK.

#### Solve the Analysis

1. Click Solve in the Workspace Toolbar.
2. Attention: Does the yellow circle and Pre-check icon have you concerned? Normally it should, we can click the Repair link to understand the issue. In this case, it is because we didn't define contacts. Since the defaults are being used, we can hit solve anyways and they are automatically calculated before solving.

3. Specify the computing location, using the radio button for On Cloud or Locally.
4. Note: Solving on the cloud consumes cloud credits.

5. Click Solve.

#### Probe the Fin Temperatures

1. Click INSPECT > Surface Probe.
2. Click the model near the edge of the fins in the higher temperature regions in a few places. Compare the samples to validate they are not outliers (indicating a possible misplaced probe).

You can see that the edge of the fins dropped by several degrees.

The improved temperature profile does come with a cost. The larger fins increase weight and material costs. Tuning your design to the right parameters may take several analyses.

You have now completed two thermal analyses, identified potential issues, and compared results between two designs.

### Thermal Stress

x/x

#### Lesson: Thermal Stress Analysis of a Disk Brake Rotor

In this exercise we'll perform a Thermal Stress analysis on a disk brake rotor. The brake rotor will be modeled using 1/8th symmetry. This has two effects:

1. A smaller model that results in faster solve times.
2. Easy application of boundary conditions on the symmetry planes.

A temperature differential will be applied to the cast iron brake rotor to simulate the thermal loads that act on the model in its operating environment. We'll examine the safety factor, heat flux, and stresses acting on the model as a result of these thermal loads.

#### Open the Brake Rotor Model

In the Samples section of your Data Panel, browse to:

Basic Training > 11 - Simulation > BrakeRotor

1. Click the Show Data Panel icon at the top of the screen, if the Data Panel is not currently shown. The Data Panel appears at the left side of the program window.
2. The top level (home view) of the Data Panel is divided into two subsections - PROJECTS and SAMPLES. Scroll to the bottom of the PROJECTS list if necessary to see the SAMPLES list.
3. Locate the Basic Training entry under SAMPLES and double-click it. The Data Panel now displays a list of the folders containing the training lesson models.
4. Click the 11 - Simulation folder.
5. Select the BrakeRotor model.

#### Save the model

When opening a sample model for the first time the active workspace in Fusion is the Modeling Workspace. The model is in Read only and needs to be saved to a personal project.

1. Click File > Save As.
2. Optionally, create a Project to store your training models.
3. a) Click New Project
b) Specify the project name
c) Press Enter.

4. Optionally, create a folder within the project to store your training models.
5. a) Click New Folder
b) Specify a folder name
c) Press Enter
d) Double-click the new folder to make it the current file saving location.

6. Click Save.

#### Access the Simulation Workspace

1. Click the workspace selection in the top left corner.
2. Select the Simulation workspace from the drop-down list.
3. Note: Notice that the toolbar changes to include commands specific to simulations.

4. Click STUDY > New Simulation Study
5. Select the Thermal Stress study type and click OK.
6. Next, we'll switch the unit system for this study to U.S.

7. Click the Edit button next to the Units node in the browser
8. Select U.S. (in.) as the unit system and click OK.

#### Apply Materials

1. Click MATERIAL > Study Materials.
2. Select Iron, Gray Cast ASTM A48 Grade 20 as the study material.
3. Click OK.

Selecting the Yield Strength as the safety factor criteria allows us to easily determine if the rotor will yield. If the safety factor falls below 1.0, the yield strength will have been exceeded and the part will begin to deform.

#### Apply Constraints

1. Click CONSTRAINT > Structural Constraint.
2. Make sure they Type is set to Fixed.
3. Select the two faces on the YZ plane of the brake rotor as shown below.
4. Activate Ux.
5. Click OK.
6. Repeat these steps, constraining the Uy direction for the two faces on the XZ plane and the Uz direction for the 8 faces on the XY plane.

2. Select the interior surface of the brake rotor as shown below.
3. Make sure Type is set to Applied Temperature.
4. Specify a temperature of 100° F.
5. Repeat these steps for the opposite end of the break rotor as shown below, applying a temperature of 400° F.

#### Adjust Mesh Settings and Solve

1. Click MANAGE > Settings.
2. Switch to the Mesh panel.
3. Drag the slider on the mesh size to the left as shown to reduce the size of the mesh.
4. Click OK.
5. Click SOLVE > Solve.
6. Choose between solve On Cloud or Locally and click Solve.

#### Review Results

1. With Safety Factor selected as the result, click INSPECT > Show Min/Max.
2. Notice that the safety factor is just larger than 1.0, indicating the rotor will not yield as a result of the applied temperature loads. Also notice that the regions of the model with the lowest safety factor are located near the edges of the notches.

To get a better understanding of why the safety factor is lowest around the edges of the notches we'll take a look at the heat flux and the stress.

1. Click INSPECT > Hide Min/Max.
2. Switch to the Heat Flux result.

Notice how the largest heat flux is located around the notches. This makes perfect sense considering the notches in the brake rotor are designed to dissipate heat.

1. Switch to the Stress result.

As we might expect, the largest stresses are located on the edges of the notch, due to the high heat flux in this region.

### Nonlinear Static Stress

x/x

#### Lesson: Support Beam with Nonlinear Material

In this exercise, we'll perform a Nonlinear Static Stress study on an aluminum beam specimen. The aluminum material is defined with nonlinear stress-strain data. The beam is loaded with a pressure load along the top surface. It is constrained using fixed supports on the bottom surface of the beam. We'll examine the stresses and the displacements that result from the applied loads and constraints.

#### Open the Support Beam Model

In the Samples section of your Data Panel, browse to:
Basic Training > 11 - Simulation > Support Beam

1. Click the Show Data Panel icon at the top of the screen, if the Data Panel is not currently shown. The Data Panel appears at the left side of the program window.
2. The top level (home view) of the Data Panel is divided into two subsections - PROJECTS and SAMPLES. Scroll to the bottom of the PROJECTS list if necessary to see the SAMPLES list.
3. Locate the Basic Training entry under SAMPLES and double-click it. The Data Panel now displays a list of the folders containing the training lesson models.
4. Click the 11 - Simulation folder.
5. Select the Support Beam model.

#### Access the Simulation Workspace

1. Click the workspace selection in the top left corner.
2. Select the Simulation workspace from the drop-down list.

Note: Notice that the toolbar changes to include commands specific to simulations.

#### Create New Nonlinear Static Stress Study

1. In the Simulation toolbar, click New Simulation Study. Notice that The New Simulation Study is the only available command at this point.
2. In the Studies dialog box, select Nonlinear Static Stress.
3. Click OK.

The rest of the simulation workspace commands are now available.

#### Copy a Material to Favorites Library

1. Click MATERIAL > Manage Physical Materials.
2. Locate the Aluminum material in the Fusion 360 Material Library (Metal > Aluminum).
3. Select the Aluminum material and add it to the Favorites Library.
4. Right-click the Aluminum material in the Favorites Library and choose Rename.
5. Change the name to Aluminum - NL.

#### Assign Nonlinear Properties to the Material

1. Switch to the Physical tab.
2. Change the Yield Strength to 386 MPa and change the Tensile Strength to 455 MPa.
3. Activate the Nonlinear check box.
4. Change the Type to Plastic.
5. Change the Initial Yield Stress to 386 MPa.
6. Click Show XY Plot.
7. Chang the unit system to ksi and enter the stress-strain data provided.
8. Click OK.
9. Click OK and close the Material Browser.

#### Assign the Material

1. Click MATERIAL > Study Materials.
2. Select the Aluminum - NL material we just created.
3. Change the Safety Factor criterion to Ultimate Tensile Strength and click OK.

#### Constrain the Beam

1. Click CONSTRAINT > Structural Constraints.
2. Make sure the Type is set to Fixed.
3. Select the two surfaces of the beam shown below and click OK.

#### Apply Forces to the Beam

2. Switch the Type to Pressure.
3. Select each of the three surfaces on the top of the beam as shown below.
4. Enter a Magnitude of 10 MPa and click OK.

#### Adjust Study Settings and Solve

1. Click MANAGE > Settings.
2. Change the Number of Steps to 100.
3. Switch to the Mesh panel.
4. Drag the slider to the left as shown below to reduce the mesh size.
5. Click OK.
6. Click SOLVE > Solve.
7. Select On Cloud and click Solve 1 Study.

#### Review the Stress Results

1. Select the Stress result from the legend.
2. Drag the step slider to see how the stresses change as the support beam is loaded.

#### Review the Stress Results

1. Click the 2D Chart icon to view the Maximum Von Mises stress throughout the load history.
2. Notice the nonlinear response of the beam. As the load increases, the beam begins to yield. If we simply ran a Static Stress study on the beam, we would only see the stresses on the beam at the end of the analysis.

3. Click Close to exit the 2D plot.

#### Review the Displacement Results

1. Select the Displacement result from the legend.

As we might expect, the maximum displacement occurs on the web of the support beam, away from the vertical supports.

You have now completed the Nonlinear Static Stress Tutorial.

### Event Simulation

x/x

#### Lesson: Event Simulation of a Snap-fit Assembly

In this exercise we'll perform an Event Simulation study on a snap-fit assembly. The assembly consists of two plastic bodies that will be pushed together. Using the Event Simulation study type, we'll simulate this behavior and examine the resultant stresses on the plastic bodies.

#### Open the Brake Snap Fit

In the Samples section of your Data Panel, browse to Basic Training>11 – Simulation>SnapFit, as follows:

1. If the Data Panel is not currently shown, click the Show Data Panel icon at the top of the screen. The Data Panel appears at the left side of the program window.
2. The top level (home view) of the Data Panel is divided into two subsections: PROJECTS and SAMPLES. Scroll to the bottom of the PROJECTS list, if necessary, to see the SAMPLES list.
3. Locate the Basic Training entry under SAMPLES and double-click it. The Data Panel now displays a list of the folders containing the training lesson models.
4. Click the 11 - Simulation folder.
5. Select the model, SnapFit.

#### Save the Model

When you open a sample model in Fusion for the first time, it appears in the MODEL Workspace. The model is read-only, and you must save a copy of it to a personal project.

1. Click File>Save As.
2. Optionally, create a Project to store your training models.
3. a) Click New Project.
b) Specify the project name.
c) Press Enter.

4. Optionally, create a folder within the project to store your training models.
5. a) Click New Folder.
b) Specify a folder name.
c) Press Enter.
d) Double-click the new folder to make it the current file saving location.

6. Click Save.

#### Access the Simulation Workspace

1. Click the workspace selection in the top left corner.
2. Select the Simulation workspace from the drop-down list.
3. Note: Notice that the toolbar changes to include commands specific to simulations.
4. Click STUDY > New Simulation Study.

Select the Event Simulation study type and click OK.

Note: You must sign up for the Fusion 360 Preview functionality and activate the advanced simulation study types to select the Event Simulation study.

#### Apply Materials

1. Click MATERIAL > Study Materials.
2. Select both bodies and change the material to ABS Plastic.
3. Click OK.

#### Constrain the Ux and Uy Directions

1. Click CONSTRAINT > Structural Constraint.
2. Make sure the Type is set to Fixed.
3. Deselect the Uz component.
4. Select the top surface of Body 1 and Body 2 as shown below and click OK.

#### Constrain the Uz Direction

1. Click CONSTRAINT > Prescribed Translation.
2. Make sure the Type is set to Displacement.
3. Select Body 1 of the assembly.
4. Deactivate Ux and Uy so that only Uz is active.
5. Enter a value of 11 mm for Uz and click OK.
6. Click the Multiplier curve icon.
7. Change the value in Row 2 of the Time column to 0.005.
8. Click OK to accept this setting and click OK again to apply the translation.
• Repeat steps 1-8, selecting Body 2 with a -11 mm displacement for the Uz component.

1. Click LOADS > Toggle Gravity On.

1. Click MANAGE > Settings.
2. Change the Total Event Duration to 0.0025 s.
3. Switch to the Mesh panel.
4. Drag the slider to the left as shown below to reduce the size of the elements.

#### Adjust Local Mesh Settings and Solve

Before we solve the simulation, we need to add some local mesh control around the smaller surfaces of the pin that will interact with the hole of the opposing body. Since this region of the assembly has most of the action in this simulation, we need a more refined mesh.

1. Click MANAGE > Local Mesh Control.
2. Select the surfaces around the pin on Body 2 as shown below. It may be helpful to hide Body 1 for this step.
3. Accept the default mesh size and click OK.
4. Click SOLVE > Solve.
5. Make sure On Cloud is selected and then click Solve 1 Study.

Note: Event Simulation studies are only available for cloud solves.

#### Review Results

1. Click the lightbulb icon next to Body 1 in the browser to Hide Body 1.
2. Click INSPECT > Show Min/Max.
3. Drag the slider in the Legend to view the Von Mises stress on Body 2 throughout the simulation.
4. Click the 2D Chart icon to view the maximum stress over the event duration.

Notice that the maximum Von Mises stress is well below the yield strength (20 MPa) for the ABS plastic. This tells us no permanent deformation will result from snapping the two bodies together.

### Shape Optimization

x/x

#### Lesson: Lightweighting of Robot Gripper Arm

This functionality is only available in Fusion 360 Ultimate.

In this exercise we'll perform a Shape Optimization study to reduce the weight of a robot gripper arm. The goal is to reduce the weight to 40% of the original design, while still maintaining a Safety Factor of at least 2.0 for the applied load. The gripper arm, made of steel, is designed to withstand compressive loads on the gripping surface.

#### Open the Gripper Arm Model

In the Samples section of your Data Panel, browse to:

Basic Training > 11 - Simulation > GripperArm Click the Show Data Panel icon at the top of the screen, if the Data Panel is not currently shown. The Data Panel appears at the left side of the program window.

1. The top level (home view) of the Data Panel is divided into two subsections - PROJECTS and SAMPLES. Scroll to the bottom of the PROJECTS list if necessary to see the SAMPLES list.
2. Locate the Basic Training entry under SAMPLES and double-click it. The Data Panel now displays a list of the folders containing the
3. Click the 11 - Simulation folder.
4. Select the Gripper Arm model.

#### Access the Simulation Workspace

1. Click the workspace selection in the top left corner.
2. Select the Simulation workspace from the drop-down list.

Note: Notice that the toolbar changes to include commands specific to simulations.

#### Create a Shape Optimization Study

1. In the Simulation toolbar, click New Simulation Study. Notice that The New Simulation Study is the only available command at this point.
2. In the Studies dialog box, select Shape Optimization.
3. Click OK.

Note: You must sign up for the Fusion 360 Preview functionality and activate the advanced simulation study types to select the Shape Optimization study.

#### Apply Constraints

1. Click CONSTRAINT > Structural Constraint.
2. Switch the Type to Pin.
3. Select the surface of each bolt hole as shown in the image below.
4. Make sure the Radial and Axial directions are constrained.
5. Click OK.

2. Set the Type to Force.
3. Select the gripping surface as shown in the image below.
4. Enter a load of 500 N.
5. Make sure the load is acting in compression (pointing toward the surface) and click OK.

#### Preserve Regions

1. Click SHAPE Optimization > Preserve Region.
2. Select the surface of the large bolt hole.
3. Adjust the diameter to 8 mm.
4. Repeat these three steps for the small bolt hole, adjusting the diameter to 5.5 mm.
5. Click OK.

#### Create Symmetry Plane

1. Click SHAPE Optimization > Symmetry Plane.
2. Select the top surface of the gripper arm.
3. Turn on Active Plane 1 and click OK.

#### Shape Optimization Criteria

1. Click SHAPE Optimization > Shape Optimization Criteria.
2. Set the Target Mass to 40%.
3. Click OK.

#### Mesh Settings

1. Click MANAGE > Settings.
2. Switch to the Mesh panel.
3. Select the Absolute Size radio button.
4. Enter a value of 1 mm.
5. Click OK.

#### Solve the Study

1. Click SOLVE > Solve.
2. Make sure On Cloud is selected and click Solve 1 Study.
3. Note: Shape Optimization studies are only available for cloud solves.

4. After the study is complete, review the results for the Load Path Criticality. Notice how the regions deemed less critical have been removed from the generated shape.

#### Promote Mesh & Modify Original Geometry

1. Click RESULTS > Promote.
2. Click SKETCH > Create Sketch.
3. Select the top surface of the gripper arm as the sketch plane.
4. Use the spline command (SKETCH > Spline) to create closed sketch objects around the material to be removed.
5. Click Stop Sketch after all of the sketches have been made.
6. Click CREATE > Extrude.
7. Select each sketch body and extrude through the thickness of the gripper arm.

#### Static Stress Study

1. Switch to the SIMULATION workspace.
2. Right-click Study 1 - Shape Optimization in the browser and select Clone Study.
3. Click MANAGE > Settings and switch to the Static Stress study type.
4. Click OK.
5. Click SOLVE > Solve.
6. Review the Safety Factor result to verify that it meets the design requirement.

You have now completed the Shape Optimization Tutorial.