XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''"> A Case Study of an Annular Plate
This example illustrates the use of Patran when there is a component having 3D geometry that is to be represented by 2D analysis geometry. In this example an annular plate is created in Patran, analyzed in MSC Nastran and postprocessed in Patran. A linear static analysis will be performed on the annular plate. Our analysis objective is to determine its maximum stress and deflection.
Problem Description
The annular plate has a concentric central hole, is simply supported at outer boundary and is subject to an annular line load as shown in
Figure 1‑1. The associated geometric, load, and material properties are described by
Table 1‑1.
Figure 1‑1 Representation of the Annular Plate
Table 1‑1 Outer Radius, a = | 20 inch |
inner Radius, b = | 5 inch |
Annular Line Load Radius, r = | 10 inch |
Line Load, W = | 1.2 lb/in |
Elastic Modulus, E = | 10E6 psi |
Poisson’s Ratio, ν = | 0.3 |
Thickness, t = | 0.125 inch |
Conceptual Model
Physically, the plate is a solid and could be modeled using solid finite elements that approximate the solution of three dimensional theory of elasticity. Conceptually, we could create a model having hundreds to thousands of elements to capture a close approximation to the exact solution. If we were to perform this analysis and critically review the results, we would find that the displacement varies linearly through the thickness and that the components of stress in the thickness direction are very small compared with the stress components in the in-plane directions.
Fortunately, S. Timoshenko and others have already made these discoveries and have employed appropriate assumptions to simplify the three dimensional theory of elasticity to a two dimensional membrane solution for in-plane behavior and a two dimensional strength of materials approximation, called Plate Theory, for the out-of-plane bending behavior.
The use of a plate representation rather than solid elements raises the question: why not use solids elements in this example? After all, with the power of Patran and MSC Nastran to create and solve large models, why bother with an approximation?
The ultimate answer is resources. With plate representation, we can obtain a solution which is sufficiently accurate for design verification using significantly fewer resources. And, with the need for rapid response to design requests for simulation, it is vitally important to minimize problem size.
Figure 1‑2 Patran Finite Element model of Annular Plate
Theoretical Solution
The theoretical solution for this case is shown below. The maximum stress at the inner edge is:
where
and W is the total applied load.
The maximum displacement is:
Case Study Task Outline
At this point we have defined the problem and conceptually established how we will model the annular plate for analysis. Next we need to map out individual modeling and analysis tasks, set up the sequence for the tasks, and specify key parameters.
To set up the framework for the project we begin with a simple checklist. In the list below, the left side identifies the parameters or tasks that are critical to the project. The right side shows the specifics that we have decided on for the analysis. These specifics will drive the project and sequence of tasks.
• Analysis Objective | Deflection/von Mises stress from load (linear-static.) |
• Model database | Annular Plate |
• Analysis Code/Type | MSC Nastran - Structural |
• Solution Type | Linear Static |
• Geometry | Created in Patran |
• Mesh Creation | IsoMesh - Quad 4 elements |
• Loads and Boundary Conditions (LBC) | Pinned Support - Line Load |
• Material Properties | Isotropic/Aluminum/Linear Elastic |
• Element Specification | 2D/Shell/Aluminum |
• Analysis | Linear static |
• Results | Results file/deformation plot/stress fringe plot |
From the checklist we have generated a Task Map that will serve as the guide for the project.
Figure 1‑3 Case Study Task Map
Analysis Procedure
Setup the Analysis Project
Creating a New Database
• On the Patran Main Menu, select File /New. The New Database Form appears.
• Enter the name annular_plate in the Filename textbox.
• Click OK.
• The New Model Preferences form appears. This form allows you to specify the generic analysis parameters for the model.
Selecting Analysis Parameters
• Set the Tolerance to Default.
• Choose MSC Nastran from the Analysis Code pull-down menu.
• Choose Structural from the Analysis Type pull-down menu and click OK.
Build the Geometry
• Creating the Base of the Annular Plate
• On the Patran Main Menu, click on the Geometry Application button.
• On the top of the Geometry form, select Action>> Create, Object>>Curve, and Method>>XYZ.
• Enter a Vector Coordinate List of <5,0,0> and Origin Coordinate List of [5,0,0]. Click Apply.
This creates a line 5 inches long in the X-direction starting from position [5,0,0].
• Change the Vector Coordinate List to <10,0,0> and the Origin Coordinate List to [10,0,0]. Click Apply. This creates Curve 2 that represents the radius of the outer ring.
• Create the Surfaces of the Annular Plate
• On the top of the Geometry form, change the Object selection from Curve to Surface, and set Method to Revolve.
• Under Sweep Parameters, enter a Total Angle of 90.0 and an Offset Angle of 0.0. Click on Curve 1 that was previously created (or type curve 1 in Curve List text box). Click Apply.
• To create Surface 2, type Curve 2 into the Curve List textbox and click Apply.
• Repeat the same procedures for Surface 1.2, 2.2, 3.2, 4.2, 6.2 and 5.2. For instance, type Surface 1.2 in the Curve List textbox and then click Apply.
Create the Finite Elements
• Create a Surface Mesh with Quad 4 Elements
• On the Patran Main Menu, click on the Elements Application button.
• On the top of Finite Element form, select Action>>Create, Object >> Mesh, Type >> Surface. Use this combination to create a surface mesh.
• Set the Value of Global Edge Length to 2. This will determine the size of our plate elements. Then, cancel the Automatic Calculation selection.
• Choose Quad4 from the Topology pull-down menu. This selects the type of element that will be used to mesh the surface geometry. The IsoMesh mesher is automatically selected below.
• Place the cursor in the Surface List textbox and then cursor select all the surfaces on the screen (or type in Surface 1:8, and click Apply).
• Because the finite elements are not connected along the geometric boundaries, we need to “sew” them together.
Equivalencing the Mesh
• On the top of the Finite Element form, select Action >> Equivalence, Object >> All, Method >> Tolerance Cube. This will equivalence the nodes along all surface boundaries.
• Click Apply.
Model the Materials
Create a Material
• On the Patran Main Menu, click on the Materials Application button.
• On the top of the Materials form, select Action >> Create, Object >> Isotropic, Method >> Manual Input.
• In the Material Name textbox, enter “Aluminum.”
• Click on the Input Properties button.
• Specify the Material Properties of Aluminum
• On the Input Options form, enter 10e6 in the Elastic Modulus databox.
• In the Poisson’s Ratio databox, enter 0.3.
• Click OK to close the Input Option form, and then click Apply on the Materials form.
Define Element Properties
Create a Property
• On the Patran Main Menu, click on the Properties Application button.
• On the top of the Element Properties form, select Action >> Create, Object >> 2D, Type >> Shell.
• In the Property Set Name textbox, enter prop_1.
• Click on the Input Properties button.
• On the Input Properties form, click in the Material Name textbox and select Aluminum from the Material Property Set list.
• Enter a shell thickness of 0.125 inch, and click OK.
• On the Element Properties form, place the cursor in the Select Members databox and then cursor select all the surfaces on the screen (or type Surface 1:8).
• Click Add and then Apply on the Properties form.
Simulate the Loads and Boundary Conditions (LBC)
Create a Distributed Load
• On the Patran Main Menu, click on the Loads/BCs Application button.
• On the top of the Loads/BCs form, select Action >> Create, Object >> Distributed Load, Type >> Element Uniform.
• In the New Set Name textbox, enter annular_load.
• Click on the Input Data button.
• On the Input Data form, enter < , ,-1.2> for Edge Distr Load and leave the Edge Distr Moment field blank. Click OK.
• Click on the Select Application Region button.
• On the Select Application Region form, under Geometry Filter, click on Geometry.
• Place the cursor in the Select Surface Edges listbox. Use the cursor to select the 4 middle surface edges from the screen. Click Add after each selection, then click OK.
Surface 7.1 1:5:2.3 should appear in the Application Region listbox.
• Click Apply on the Loads/Boundary Conditions form.
Create a Constraining Condition (Displacement)
• On the Patran Main Menu, click on the Loads/BCs Application button.
• On the top of the Materials form, select Action >> Create, Object >> Displacement, Type >> Nodal.
• In the New Set Name textbox, enter pinned.
• Click on the Input Data button.
• On the Input Data form, enter <0,0,0> for Translations and leave the Rotations field blank.
Click OK.
• Click on the Select Application Region button.
• Under Geometry Filter, click on Geometry.
• In the Select menu, click on the Edge option.
• Place the cursor in the Select Geometric Entities databox. Use the cursor to select the 4 outer surface edges on the screen. Click Add after each selection, then click OK. Surface 2:6:2.3 7.3 should be the edges selected.
• Click Apply on the Loads/Boundary Conditions form.
• Rotate to Iso3 view.
Create MSC Nastran Input File
Create the MSC Nastran Input (Bulk Data) File and Run the Analysis
• On the Patran Main Menu, click on the Analysis Application button.
• On the top of the Analysis form, select Action >> Analyze, Object >> Entire Model, Method >> Full Run.
• Click on the Solution Type button.
• On the Solution Type form, select Linear Static. Click OK.
• Click Apply on the Analysis form.
• The analysis will take a few seconds before finishing depending on the speed of your computer. A file by the name annular_plate.bdf is created and submitted to MSC Nastran. This assumes proper configuration of the P3_TRANS.INI file (Windows) or the site_setup file (Unix), which point Patran to the proper location of the MSC Nastran executable.
Retrieve the Analysis Results
Translate the Results into Patran for Results Postprocessing
• On the top of the Analysis form, select Action >> Attach XDB, Object >> Result Entities, Method >> Local.
• Click on the Select Results File button.
• On the Select File form, select annular_plate.xdb. Click OK.
• Click Apply on the Analysis form.
Results Postprocessing
Create Fringe and Deformation Plot
• On the Patran Main Menu, click on the Results Application button.
• On the top of the Result form, select Action >> Create, Object >> Quick Plot.
• In the Select Result Cases window, select Default, Static Subcase.
• In the Select Fringe Result window, select Displacement, Translational.
• In the Select Deformation Result window, select Displacement, Translational.
• Click Apply.
