1 / 14

DINÂMICA ESTRUTURAL Prof. Airton Nabarrete

DINÂMICA ESTRUTURAL Prof. Airton Nabarrete. Cap. 7: MEF – Parte 1. EST - 56. Programa. Modelagem Dinâmica Estrutural em Patran/Nastran Análise de Freqüências Naturais em Asa de Aeronave. Step 1. Create a New Database for 1D Element Model. a. d.

aliya
Télécharger la présentation

DINÂMICA ESTRUTURAL Prof. Airton Nabarrete

An Image/Link below is provided (as is) to download presentation Download Policy: Content on the Website is provided to you AS IS for your information and personal use and may not be sold / licensed / shared on other websites without getting consent from its author. Content is provided to you AS IS for your information and personal use only. Download presentation by click this link. While downloading, if for some reason you are not able to download a presentation, the publisher may have deleted the file from their server. During download, if you can't get a presentation, the file might be deleted by the publisher.

E N D

Presentation Transcript

  1. DINÂMICA ESTRUTURALProf. Airton Nabarrete Cap. 7: MEF – Parte 1 EST - 56

  2. Programa • Modelagem Dinâmica Estrutural em Patran/Nastran Análise de Freqüências Naturais em Asa de Aeronave

  3. Step 1. Create a New Database for 1D Element Model a d Create a new database for 1D element model. • File / New. • Enter cant_beam_1D as the file name. • Click OK. • Choose Default Tolerance. • Select MSC.Nastran as the Analysis Code. • Select Structural as the Analysis Type. • Click OK. e f b c g

  4. Step 2. Create Curve Geometry d a • Geometry: Create / Curve / XYZ. • Select on Vector Coordinates List and enter < 1 0 0 >. • Apply. • Change view to Iso 1 View. b c

  5. Step 3. Create 1D Element Mesh • Elements: Create / Mesh / Curve. • Topology: Bar2. • Click on Curve List and select the curve. • Enter 1 for Global Edge Length. • Apply. a c b c d e

  6. Step 4. Apply Constraints a • Loads / BCs: Create / Displacements / Nodal. • Select on New Set Name: and enter apoio. • Select Input Data. • Enter < , 0, 0> for Translations <T1 T2 T3 >. • OK. • Click on Select Application Region. • Select FEM for Geometry Filter. • Click on Select Nodes and select Node 2. • Add. • OK. • Apply g d h i b j c e f

  7. Step 4. Apply Constraints (cont.) a • Loads / BCs: Create / Displacements / Nodal. • Select on New Set Name: and enter apoiofixo. • Select Input Data. • Enter < 0, 0, 0> for Translations <T1 T2 T3 >. • OK. • Click on Select Application Region. • Select FEM for Geometry Filter. • Click on Select Nodes and select Node 1. • Add. • OK. • Apply g d h i b j c e f

  8. Step 5. Create Material Properties a • Materials: Create / Isotropic / Manual Input. • Select on Material Name and enter aco. • Select Input Properties. • Enter: Elastic Modulus: 2e11. Poisson Ratio: 0.3 Density: 7860. • OK. • Apply. d b c e f

  9. Step 6. Create Element Properties for the 1D Beam Topology a • Properties: Create / 1D / Beam. • Option(s): General Section / Standard Formulation. • Select Property Set Name and enter viga. • Select Input Properties. • From the Material Property Sets, select aco for Material Name. • Select Create Sections Beam Library. e c b f d

  10. Step 6. Create Element Properties for the 1D Beam Topology (Cont.) • In New Section Name: retangular. • Select the rectangular cross-section button and enter: W= 0.05, H = 0.05. • Calculate / Display. • OK. • Enter < 0 1 0 > in Bar Orientation. • OK. • Click on Select Members and select Curve 1. • Add. • Click Apply. • Display the cross-section to scale under Display / Load/BC /Elem. Props… using Beam Display / 3D: FullSpan + Offsets. • Click Apply. b a e b c Notice that the name “retangular” now appears in the Input Properties form under Section Name. Area, Inertia and Torsional Constant have values. The values are ghosted out so that to change them it is necessary to use the Create Section button. d f

  11. Step 6. Create Element Properties for the 1D Beam Topology (Cont.) • This is the entire 1D model. A representation of the cross-section is shown, even though the geometry is only 1D.

  12. Step 7. Run Analysis for 1D Beam a • Analysis: Analyze / Entire Model / Full Run. • Select Solution Type. • Choose NORMAL MODES for Solution Type. • OK. • Apply. c d b

  13. Step 8. Read Results Under Analysis a Attach the .xdb file to read the results. • Analysis: Access Results / Attach XDB / Result Entities. • Click on Select Result File. • Select and attach the viga.xdb. • OK. • Apply. c d b e

  14. Step 9. View Results a Create a Deformation plot . • Results: Create / Deformation. • Select Results icon. • Select Default, A1:Mode 1: Freq = 126.94 under Select Result Cases. • Select Eigenvectors, Translational under Select Deformation Result. • Show As: Resultant. • Apply. b c d e

More Related