Laboratory 4 - Procedure¶
In this lab, you will develop a model of your cantilevered beam using Ansys, and conduct a modal analysis to discover its fundamental frequencies and mode shapes. You will be judging the accuracy of your model in three ways:
Convergence - examining the tendency of the FEA to approach a final solution with decreasing element size
Verification - comparing your results to an analytical model (the frequencies you calculated in Lab 3)
Validation - comparing your results to an experimental model (the frequencies you measured in Lab 3 using FFT analysis)
Task 0 - Getting started (20-30 minutes)¶
Read through the Background and Resources document for this lab.
Open Ansys Workbench on your lab computer and get familiar with its interface. Poke around and take a look at different menus.
Click “Help” -> “Getting Started” and read through the instructions that appear.
TAs will not answer your questions until you have completed Task 0
Task 1 - Define your FEA model (45-60 minutes)¶
First, you will create a rectangular beam with the same material properties and dimensions as the one you used in Labs 2 and 3.
In Ansys Workbench, create a new project.
To select a modal analysis, drag the “Modal” option from the left-hand menu into the project schematic.
Double-click on “Engineering Data” to specify the material you will use for your beam.
Click “Engineering Data Sources” (up top, by the tabs) then select “general materials” from the materials library.
Find your material, and add it to your model using the yellow plus sign.
Exit the library by clicking on “Engineering Data Sources” one more time.
Select your material to edit its properties in the bottom pane. Make sure the values for Young’s modulus and density match the values you used for Lab 3.
Close the tab to return to the project schematic.
Right-click on “geometry” and open a new SpaceClaim file. Here you can define the geometry of your beam.
Sketch a rectangle on the xy, yz, or xz plane.
Dimension the rectangle to match the cross-section of your beam
Using the “extrude” tool, extrude your sketch to match the length of your beam.
Save the model, and return to the main Workbench window.
Next, you will define the specifics of the analysis.
Double-click on “Model” in the project schematic. Ansys Mechanical will load in a new window.
The top left pane is the “Project tree”. Here, all the elements of your model are accessible.
Click the plus sign next to “Geometry” to expand it, and select your solid by clicking on it. All of its properties will appear in the “Details” pane below. Under “Material”, make sure your solid is using the material you defined earlier.
You will need to define the boundary condition for your beam. Right-click on “Modal” in the Project Tree, and “insert” a “fixed support”. Select one end-face of your beam with a left-click, then press “Apply” in the details pane.
Next, you will configure the mesh that is made up by the nodes of the model. Click on “Mesh” in the Project Tree, and take a look at the details pane.
Expand “Sizing”, and turn “Use Adaptive Sizing” to No.
Expand “Default”, and set “Element Order” to Linear.
Still in “Default”, set your “Element Size”. This will dictate the number of elements, and therefor nodes, in your model. As a (low) starting point, set it to the width of your beam.
Right-click “Mesh” in the Project Tree, and select “generate”. You should see your mesh applied to your model.
Expand “Statistics” in the details pane for your mesh. It will show the number of nodes and elements in your model.
Task 2 - Run your initial analysis (10-15 minutes)¶
Right-click “Solution” and select solve. After it completes, you will see the results plotted and tabulated in the bottom two panes.
You will first need to determine which modes correspond to the modes you measured in Lab 3 (Refer to Background and Resources).
Click and drag to highlight all 6 mode shapes in the “Tabular Data” pane. Right-click and select “Create mode shape results”. This will add several “Total Deformation” results to your Solution in the Project Tree. Right-click to evaluate and display them.
By inspection and by comparison of frequencies, determine which mode shapes correspond to the ones measured in Lab 3. These are the frequencies we are interested in. (Refer to the Background and Resources section of Lab 3 for a depiction of mode shapes).
Make a note of the natural frequencies and the number of nodes.
Task 3 - Adjust your analysis to find convergence (30-45 minutes)¶
Change the number of nodes by setting a different Element Size in the Mesh detail pane. You will need to right-click on “Mesh” and select “update” to get the model ready to solve.
Gradually decrease the element size (i.e., increase the number of nodes). As described in the Background and Resources section, you will see the relative error and absolute error converge on final values.
Repeat this process until you have seen convergence of the three natural frequencies you measured in Lab 3.
Your Report¶
Demonstrate convergence of the first three modes, using the two methods shown in the Background and Resources section.
What was your hypothesis for this investigation?
Compare your FEA results to your experimental and analytically predicted results. Do they agree? How does this affect your hypothesis? What can you conclude from the results?