Pre-stressed Modal Analysis Winter Semester

2 Goals Our goal is to simulate the modal response of the tension link (shown below) in both a stressed and unstressed state. Specifically, we will load the link with a 4000 N tensile load and compare the natural frequency to that of the unloaded component.

3 Start Page From the launcher start Simulation. Choose “ Geometry > From File... “ and browse to the file “ tension_link.x_t ”.

4 Choose the Metric mm unit system. “ Units > Metric (mm, kg, N, C, s) Highlight the Model branch, RMB and “ Duplicate ”. Rename the 2 Models branches as shown. RMB > Rename Preprocessing 3

5 “ Unstressed ” modal analysis Choose “ Modal ” analysis under “ New Analysis ” menu start

6 “ Unstressed ” modal analysis Highlight the Modal branch and add supports as described here: Select one of the inside faces of one washer “ RMB > Insert > Fixed Support ”. Select the face on the rim of the other washer “ RMB > Insert > Frictionless Support ”. Solve the model

7 Results  Highlight the solution branch  Open the Tabular Data (bottom of the page) and select all the modes  RMB  Create Mode Shapes  List of 6 Total Deformation results will appear under the solution branch.  Each result represent one mode  RMB on the solution branch  Evaluate All Results

8 “ Pre-stressed ” modal analysis Under Prestressed branch: Add ‘ Static Structural ’ analysis under “ New analysis ” menu, to calculate the pre- stressing. Apply supports to the model: Highlight one of the inside faces of one washer “ RMB > Insert > Fixed Support ”. Highlight the face on the rim of the other washer “ RMB > Insert > Frictionless Support ”.

9 Apply tensile load to the model Orient the model as necessary and zoom in on the inside face of the washer where the frictionless support is applied to the rim. Highlight its inside surface “ RMB > Insert > Force ”. Enter “ 4000 ” in the Magnitude field [N]. Note use the “ Direction ” field to modify the force direction if necessary to insure the load is tensile (see below). Direction filed

10 Preprocessing Set analysis options to run a pre-stressed modal analysis next: Highlight Analysis Settings Expand the “ Analysis Data Management ” section Change “ Future Analysis ” to “ Pre-stressed Analysis ” Solve the Static Structural analysis: Highlight the Static Structural  RMB  Solve Note : If “ Future Analysis ” is not set, then the “ Static Structural ” analysis will have to be re-run

11 Post-processing Insert deformation and stress results and review the solution from the structural analysis: Total Deformation on tension link Equivalent Stresses on tension link

12  Add Modal analysis from the “ New Analysis ” Menu.  Note:  Note: The aim of the static structural analysis is to set the pre-stress conditions. Therefore, the modal analysis ’ s initial condisition shall use the static structural analysis results. Create a Pre-Stressed Modal analysis

13  Highlight the “ Initial Conditions ” branch under the Modal branch  In the details window set the ‘ Initial Condition Environment ’ to Static Structural Note: Another way of inserting the Pre-Stressed Modal Environment after the Structural solve is to insert a result item (e.g: Total Deformation) and RMB on the result item > “ Create Modal Analysis with Pre-Stress ” Create a Pre-Stressed Modal analysis

14 Solve  Highlight the Modal branch and solve

15 Evaluate the results  Highlight the solution branch  Open the Tabular Data (bottom of the page) and select all the modes  RMB  Create Mode Shapes  List of 6 Total Deformation results will appear under the solution branch.  Each result represent one mode  RMB on the solution branch  Evaluate All Results

16 Post-processing  When the solutions are completed, highlight the first mode shape (the first Total deformation result) and review the results from each model. Unstressed Pre-stressed

17 Post-processing  As shown below the prestressed results should show an increase in frequencies. Note: the actual frequencies may vary slightly from those shown due to meshing and machine differences. Unstressed Pre-stressed

18 Post-processing  Although not a requirement, good practice recommends that we include a stress calculation in our pre-stressed branch to insure that the component does not fail due to the applied load.  By comparing the reported stresses to the material ’ s yield values (Engineering Data) we can assess the component ’ s performance with respect to the applied load.

19 Post-processing  Highlight the Equivalent Stress branch, note that the max stress magnitude is 98.2MPa  Open the Engineering Data for Structural steel  Note that the stress value is to low regarding the steel yield strength (250MPa).