Simcenter 3D Solutions Pre-Stressed Modal Analysis of a Guitar String tutorial - Part 4/4 - Apply boundary conditions, solve and postprocess the model

Summary

In this tutorial, a simple simulation of a guitar string will be used to illustrate the process of performing a prestressed modal analysis in Simcenter 3D. This tutorial is divided into 4 parts: 1. Introduction and equation for hand calculation 2. Guitar string Geometry creation and setup SIM and FEM files 3. Mesh and assign material properties to Guitar string 4. Apply boundary conditions, solve and postprocess the model

Details

Please follow the previous parts of this tutorial here:
Pre-Stressed Modal Analysis of a Guitar String tutorial - Part 1/4 - Background
Pre-Stressed Modal Analysis of a Guitar String tutorial - Part 2/4 - Guitar string Geometry creation and setup SIM and FEM files
Pre-Stressed Modal Analysis of a Guitar String tutorial - Part 3/4 - Mesh and assign material properties to Guitar string

Step 07: Constrain the String


•Double click the Guitar_String_sim1 part in the Simulation File View pane using the left mouse button
•Select Fixed Constraint from the Constraint Type drop-down menu in the Loads and Conditions group of the Home tab tool ribbon
•Select the nodes on the two ends of the string (use the Type Filter in the top left corner to select nodes)
•Click OK

Step 08: Run the Analysis on the Non-Pre-stressed String

•Right click on Solution 1 in the Simulation Navigator and select Solve

•Click OK

•Once the Analysis Job Monitor reports that the analysis has been completed, click Cancel on that window and then close the Information window

Step 09: Post the Modal Results for the Non-Pre-stressed String

•Expand the Results item in the Simulation Navigator

•Double click on the Structural Item

•Expand the Structural item in the Post Processing Navigator and then Mode 1, 5.07776Hz

•Double click on Displacement – Nodal

•The first mode shape is now displayed

•Notice how much lower in frequency this is than the 196Hz associated with a correctly tuned G or 3rd string

Step 10: Animate the Mode Shape

•Select Animate     in the Animation group of the Results tab tool ribbon

•Set the Style to Modal

•Set the Number of Frames to 20

•Check the Full-cycle checkbox

•Press Play

•When the string vibrates in the mode depicted, a sound at a pitch of about 5.265Hz will be heard

When done viewing the mode, click Stop and then Cancel

Step 11: Create the Static Solutions Subcase

•Click Return to Home

•Right-click on Solution 1 and select New Subcase…

•In the Solution Step menu, ensure that Step is set to Subcase – Statics

•Click on Create Step

•Click OK

•Create another subcase using the same process as mentioned above

•Set Relative Position to [Before] Subcase – Statics 1

•Click OK

Step 12: Create the String Pretension using the Bolt Pre-Load Tool

•Select Bolt Pre-Load from the Load Type drop-down menu in the Loads and Conditions group of the Home tab tool ribbon

•Ensure that the drop-down at the top of the Bolt Pre-Load menu is set to Force or Displacement on 1D Elements

•Set the Force to 92.05N

•Select a single element (use the Type Filter in the top left corner to select elements) and click OK

Step 13: Run the Analysis on the Pre-Stressed String


 

•Right click on Solution 1 in the Simulation Navigator and select Solve

•Click OK

•Once the Analysis Job Monitor reports that the analysis has been completed, click Cancel on that window and then close the Information window

Step 14: Post the Modal Results for the Pre-Stressed String

•Expand the Results item in the Simulation Navigator

•Double click on the Structural Item

•Expand the Structural item in the Post Processing Navigator, then Subcase – Eigenvalue Method 1

•Double click on Displacement – Nodal

•The first mode shape is now displayed

•Notice that the mode frequency has increased to 198.74Hz, which is close to the predicted value of 196Hz