Simcenter 3D Solutions Chladni Plate - Normal Mode Analysis - Part 2/5 - How to create Chladni Plate geometry and setup FEM and SIM files

Summary

This tutorial shows how to analyze normal modes on Chladni plate using Simcenter 3D. This tutorial is divided into 5 parts: 1. Background of the Chladni plate 2. How to create Chladni Plate geometry and setup FEM and SIM files 3. Mesh and assign material properties to Chladni plate 4. Apply boundary conditions to Chladni plate 5. Run and postprocess the normal mode results

Details

For previous steps - please follow below tutorial
Chladni Plate - Normal Mode Analysis - Part 1 - Background

Part 2 : How to create Chladni Plate geometry and setup FEM and SIM files

Step 01: Create a Simcenter Part Model

•Launch a new session of Simcenter

•File > New

•In the window that appears, select Model from the list of Templates

•Set the Name to Plate.prt

•Choose a suitable directory where the model will be saved

Click OK

Step 02: Create the Plate Geometry

•Select Extrude

•Click on the XY plane to start the creation of a sketch

•Select Rectangle

•Draw a rectangle and use Rapid Dimension to place the indicated dimensions on the sketch

•Click Finish        to exit the sketch environment

•Set the Start and End limits of the Extrude to 0mm

•Click OK

Step 03: Create the SIM and FEM


 

•File > Pre/Post

•Click New FEM and Simulation button     (typically in the top left corner)

•The menu shown to the right should appear

•Ensure that the Create Idealized Part checkbox is ticked. This will enable clean-up operations to be performed without changing the geometry that was imported

•Click OK

Step 04: Set the Solution Parameters for the Analysis

•The menu that appears allows various solution parameters to be set. Check that:

•Solver is NX Nastran

•Analysis Type is Structural

•Solution Type is SOL 103 Real Eigenvalues

•The default settings will suffice for this analysis. If necessary, it is possible to modify these settings at a later stage in the model setup process

•Click OK

•Click OK in the Solution Step menu that appears. These settings will be adjusted later

Step 05:


Inspect the Simulation Navigator

•Expand all items in the Simulation Navigator

•Observe the positions of the SIM (.sim), FEM (.fem), Idealized Part (_i.prt) and the Part (.prt) in the Navigator

•Ensure that the Simulation File View at the bottom of the Simulation Navigator is expanded as this will make it easier to navigate between the different simulation files

•Double click the Plate_fem1_i part in the Simulation File View pane using the left mouse button. An Idealized Part Warning message should appear

•Click OK

Step 06: Promote the Bodies to the Idealized Part


 

•Click on the Promote button 

•Select the plate in the display port

•Click OK

Step 07: Split the Plate to Ensure that there is a Node at the Center

•Select the Split Body       tool in the Geometry Preparation group of the Home tab tool ribbon

•Select the plate and click the middle mouse button

•Set the Tool Option to New Plane

•Set the plane type to Point and Direction       in the Specify Plane drop-down menu

•Select the midpoint on one of the edges of the plate as shown in the adjacent image and click Apply

•Repeat this process so that the plate is split into four equally sized sections

Step 08: Stitch the Plate Edges

•Double click the Plate_fem1 part in the Simulation File View pane using the left mouse button

•Select the Stitch Edge       tool in the Polygon Geometry group of the Home tab tool ribbon

•Ensure that Method is set to Automatic

•Set Geometry to Stitch to Edge to Edge

•Set the Search Distance and Snap Ends Tolerances to 0.1mm

•Select all bodies in the display

Click OK

Please follow Chladni Plate - Normal Mode Analysis - Part 3 - Mesh and assign material properties to Chladni plate