XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''"> A Case Study of a Lug
In lieu of constructing new models from scratch, Patran supports direct interfaces to all major CAD systems. This added feature of using an existing CAD geometry model minimizes repetitive modeling efforts and ensures better accuracy between a CAD design model and its intended analysis model.
Problem Description
This lug model is simply supported at the bottom and is subject to a quadratic contact load as shown by
Figure 4‑7. The associated geometric, load, and material properties are described by
Table 4‑1.
Figure 4‑7 Loads on the Lug
Table 4‑1 Properties of the Lug
Elastic Modulus, E = | 10E6 psi |
Poisson’s Ratio, ν = | 0.3 |
Contact Load | 12.5*(|x|-2)**2 |
Conceptual Model
Unlike the case study of the annular plate where we idealized the solid model with two dimensional approximation, this example illustrates the versatility of Patran in handling arbitrary solids. We import the existing Parasolid geometry into our database as the foundation of our analysis, utilize the highly automated Tetmesh approach to generate appropriate three dimensional elements, and incorporate all relevant functional assignments (materials, properties and loads/boundary conditions) to complete our analytical model.
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 lug in the Filename textbox.
• Click OK.
• The New Model Preferences from appears. This form allows you to specify the generic analysis parameters for the model.
Selecting Analysis Parameters
• Set the Tolerance to Default.
• Choose MD Nastran from the Analysis Code pull-down menu.
• Choose Structural from the Analysis Type pull-down menu and click OK.
Import the Geometry
Importing a Parasolid Geometry
• On the Patran Main Menu, select File >> Import.
• The Import form appears.
• On the Import form, select Source >> Parasolid xmt, and then click on the Parasolid xmt Options.
• From the Option form, select Model Units button. Change the unit to 39.37(Inches) under the Model Unit Override window. Click OK to return to the Option form, and click OK one more time to return to the Import form.
• Select the lug.xmt in the Filename field and click Apply.
• Now change the view to Isoview 1 by clicking on the Isoview1 button on the Main menu. Also, turn ON the Display Line Icon.
Create a New Coordinate System
• On the Patran Main Menu, click on the Geometry Application button.
• At the top of the form, select Action >> Create, Object >> Coord, Method >> 3Point.
• Change the Coord ID List to 99. Enter Origin = [3,6,0], Point on the Axis 3 = [3,6,1], and Point on Plane 1-3 = [4,6,1]. Click Apply.
Create the Finite Elements
Create a Solid Mesh with Tet10 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 >> Solid. Use this combination to create a solid mesh.
• Change the Global Edge Length to 0.4 and cancel the selection, Automatic Calculation.
• Select TetMesh in the Mesher field.
• Using the Element Topology pull-down menu, highlight Tet10. This selects the type of element that will be used to mesh the solid geometry.
• Place the cursor in the Input List textbox and cursor select both solids (or type in Solid 1 2). Click Apply.
Equivalencing the Mesh
• On the top of the Finite Element form, select Action >> Equivalence, Object >> All, Method >> Tolerance Cube. This will equivalence all the nodes.
• 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 “steel.”
• Click on the Input Properties button.
• Specify the Material Properties of Steel
• On the Input Options form, enter 30e6 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 the Element Properties
• On the Patran Main Menu, click on the Properties Application button.
• On the top of the Properties form, select Action >> Create, Object >> 3D, Type >> Solid.
• 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 listbox and select steel from the Material Property Set list. Click OK.
• On the Element Properties form, click on the Select Members textbox. Select and Add all the geometry entities.
• Click OK to close the Input Properties form, and then click Apply on the Properties form.
Create a PCL Function Representing the Loading Condition
• On the Patran Main Menu, click on the Fields Application button.
• On the top of the Loads/BCs form, select Action >> Create, Object >> Spatial, Method >> PCL cellheadwhite. Name the Set quadratic_loading, and select Vector as the Field Type.
• Select Real for the Coordinate System Type and enter Coord 99 in the Coordinate System textbox.
• In the second component field, enter the equation 12.5*(abs(‘x)-2.)**2.
Make sure all the integers have a decimal point.
• Click Apply.
Simulate the Loads and Boundary Conditions (LBC)
Create a Load Based on the PCL
• On the Patran Main Menu, click on the Loads/BCs Application button.
• On the top of the Loads/BCs form, select Action >> Create, Object >> Force, Type >> Nodal. Name the Set Contact_load, and click on the Input Data button.
• On the Input Data form, click in the Force databox and then select the quadratic_loading inside the Spatial Field databox. 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 Geometric Entities databox. Next, use the cursor to select the bottom face of the top solid from the screen (or type in Solid 2.3). Click Add and then click OK.
• Click Apply in the Loads/Boundary Conditions form.
Create a Displacement
• On the Patran Main Menu, click on the Loads/BCs Application button.
• On the top of the Loads/BCs form, select Action >> Create, Object >> Displacement, Type >> Nodal.
• Name the set support.
• 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.
• On the Select Application Region form under Geometry Filter, click on Geometry.
• Place the cursor in the Select Geometric Entities databox. Next, use the cursor to select the bottom face of the bottom solid from the screen (or type in Solid 1.3).
• Click Add, and then click OK.
• Click Apply on the Loads/Boundary Conditions form.
Run MD Nastran
Create the MD Nastran Input (Bulk Data) File
• On the Patran Main Menu, click on the Analysis Application button.
• On the top of the Analysis form, select Action >> Analysis, 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. A file by the name lug.bdf is created and submitted to MD 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 MD Nastran executable.
• Translate the Results into Patran for Results Postprocessing
• On the top of the Analysis form, select Action>>Access Results, Object>>Attach XDB, Method>>Result Entities.
• Click on the Select Results File button.
• On the Select File form, select lug.xdb. Click OK.
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 listbox, select Default, Static Subcase.
• In the Select Fringe Result listbox, select Stress Tensor.
• In the Select Deformation Result listbox, select Displacement, Translational.
• Click Apply.
