Tutorial de exemplos de aplicação do software ABAQUS, Manuais, Projetos, Pesquisas de Projeto Estrutural e Arquitetura

Baixe Tutorial de exemplos de aplicação do software ABAQUS e outras Manuais, Projetos, Pesquisas em PDF para Projeto Estrutural e Arquitetura, somente na Docsity!

UNIVERSIDADE DE S ÃO PAULO

E SCOLA DE E NGENHARIA DE S ÃO CARLOS

E NGENHARIA AERONÁUTICA

TUTORIAIS ABAQUS

PROF. DR. VOLNEI T ITA

INDEX

• 1. AERONAUTICAL STRUCTURES ANALYSIS............................................................................
  • 1.1. ABAQUS
  • 1.2. TUTORIAL 01 – CANTILEVER B EAM
  • 1.3. TUTORIAL 02 – B AR TRUSS
  • 1.4. TUTORIAL 03 – TRACTION ANALYSIS
  • 1.5. TUTORIAL 04 – B RACKET
  • 1.6. TUTORIAL 05 – ANALYSIS K T
  • 1.7. TUTORIAL 06 – CONTACT
  • 1.8. TUTORIAL 07 – COMPOSITE M ATERIAL
  • 1.9. TUTORIAL 08 – H EAT TRANSFER
  • 1.10. TUTORIAL 09 – SANDWICH STRUCTURES
  • 1.11. TUTORIAL 10 – ELASTIC-P LASTIC ANALYSIS...........................................................................
  • 1.12. TUTORIAL 11 – ANALYSIS M ODAL
  • 1.13. TUTORIAL 12 – ANALYSIS DYNAMICS
  • 1.14. TUTORIAL 13 – I NTRODUCTION P YTHON
  • 1.15. TUTORIAL 14 – I NTRODUCTION UMAT
  • 1.16. TUTORIAL 15 – DAMAGE M ODEL - UMAT
  • 1.17. TUTORIAL 16 – I NTRODUCTION VUMAT

 ABAQUS/CAE AND ABAQUS/VIEWER

Abaqus/CAE is a complete Abaqus environment that provides a simple, consistent interface for creating, submitting, monitoring, and evaluating results from Abaqus/Standard and Abaqus/Explicit simulations. Abaqus/CAE is divided into modules, where each module defines a logical aspect of the modeling process; for example, defining the geometry, defining material properties, and generating a mesh. As you move from module to module, you build the model from which Abaqus/CAE generates an input file that you submit to the Abaqus/Standard or Abaqus/Explicit analysis product. The analysis product performs the analysis, sends information to Abaqus/CAE to allow you to monitor the progress of the job, and generates an output database. Finally, you use the Visualization module of Abaqus/CAE (also licensed separately as Abaqus/Viewer) to read the output database and view the results of your analysis. Abaqus/Viewer provides graphical display of Abaqus finite element models and results. Abaqus/Viewer is incorporated into Abaqus/CAE as the Visualization module. A complete Abaqus analysis usually consists of three distinct stages: preprocessing, simulation, and postprocessing. These three stages are linked together by files as shown below:

Figure 1 – Flowchart of the complete analysis with Abaqus (FONTE: Abaqus Documentation 2010)

 COMPONENTS OF THE MAIN WINDOW

You interact with Abaqus/CAE through the main window, and the appearance of the window changes as you work through the modeling process. Figure 1 shows the components that appear in the main window. The components are:

Figure 2 – Components of the main windows (FONTE: Abaqus Documentation 2010)

Figure 3 – Organization of a model defined in terms of an assembly of part instances. (FONTE: Abaqus Documentation

Figure 4 – Allowable references between levels (FONTE: Abaqus Documentation 2010)

 UNITS

Before starting to define this or anymodel, you need to decide which system of units you will use. Abaqus has no built-in system of units. Do not include unit names or labels when entering data in Abaqus. All input data must be specified in consistent units. Some common systems of consistent units are shown.

Figure 5 – Consistent Unit (FONTE: Abaqus Documentation 2010)

The SI system of units is used throughout this guide. Users working in the systems labeled “US Unit” should be careful with the units of density; often the densities given in handbooks of material properties are multiplied by the acceleration due to gravity.

From Figure 7(b), assuming the hypothesis that θ is small and that the flat sections before loading remains plane after loading, it arrive at the following relationship:

y dx

y

tg θ ≈θ=∆ dx ⇒θ =∆

Deriving with respect to x and it’s knowing that θ is the first derivative of v(x) (Figure 7(a)) cames the following relationship:

ddx θ y = ∆ dxdx ⇒ v "( x ) y = ε

Assiming a lineat distribuition of strain in the section (Figure 7(a)), it has the moment is: M ydsy Ky ds KI ∫ s ∫ s

= σ( ) =^2 =

Isolating K in the previous equation and back in the equation of moment, it has:

σ = MI y

(a) (b) Figure 8 – Stress distribution

From constitutive equation σ = Eε, substituting the relations for the stress (σ) and strain (ε), deduced above, it’s arrives at the following relationship:

EI

v "= M ( x )

Particularization to the case of cantilever beam, it has the equation of moment at the bar: M ( x )= F ( l − x )

The boundary conditions are v ( (^) x = 0 )= 0 and v ' (^) ( x = 0 )= 0 , it arrives at the following equation

for the elastic line of the cantilever beam:

= ^ −

2 x^3

lx

EI

v F

In the end of x = l, it has:

EI

v Fl

3

For implementation in numerical methods there are several ways to make the energy balance calculation and the variational principle of virtual work, here called PTV. In the bar or truss elements using the finite element method, it is best understood using an original approach for teaching the PTV. For a bar element with axial force only (lattice), it follows that the PTV is given by the following equation:

∫ V ∂ =∫ ∂ + ∂

l

Eu udv q udx Pul

0

Eu udsdx q udx Pul u

l l s ∫ ∫ ∂^ =∫ ∂ + ∂^ ∀∂ 0 0

Using the same polynomials (FEM) to approximate the virtual displacement ( ∂ u ) and actual (u) (Galerkin) and considering that the area is uniform, comes the following equation for this problem.

∫ = ∫ +

l T l

ES dxu q dx P l

0 0

Where it has the stiffness matrix is given by the equation:

= ∫

l

Kij ES i j dx

0

Can be observed that it is necessary that the functions have at least approximating the first derivative. The force vector by the equation:

 PROBLEM D ESCRIPTION

Properties:  Material: Al7475-T6 (see properties in MIL-HDBK-5J)  E = 10.3×10^3 ksi (71016MPa)  ν = 0.

The model will be a bar clamped with dimension of the 5000. WARNING: At this point it is important to mention the issue of dimensional consistency. There is no predefined system of units within Abaqus, so the user is responsible for ensuring that the correct values are specified. Here it uses SI units (See Figure 5).

H1 H

W

t

Section 1 W = 200 mm t = 1.8 mm H1 = 184 mm H2 = 200 mm

 GEOMETRY

1. Start Abaqus and choose to create a new model database.
2. Select “Part” in the Module.
3. In the Create Part dialog box name the part and a. Name “Beam” b. Select “3D” c. Select “Deformable” d. Select “Wire” e. Set approximate size = 10.000 (Not important determines size of grid to display) f. Click “Continue…” g. Create the sketch shown below

 PROPERTIES

1. Change Modules. In the Module drop-down box beneath the Tool Bar, select “Property”.
2. Material definition (Isotropic).
3. Material Manager → Create

a. Name the new material “Material-1” and give it a description if you want. b. Click on the “Mechanical” → “Elasticity” → “Elastic”. c. Define Young’s Modulus (71016) and Poisson’s Ratio (0.33).

3. Profile Manager → Create
4. Create Profile… a. Name the Profile and select “I” for the shape. b. Click “Continue”… c. Enter the values for the profile shown below… d. Clic “Ok”.

e. Select the material create above (Material-1) f. Click “Ok”

8. Create Assignment Manager → Create…
9. Assignment Manager… a. Click “Create…” b. Select the entire geometry in the viewport c. Click “Done” d. Select the section create above (BeamProperties) e. Click “Ok”.

10. On the toolbox area → Click on the “Assign Beam Orientation” icon… a. Select the entire geometry in the viewport b. Click “Done” in the view port c. Accept the default value of the approximate n1 direction → “Enter” d. Click “Ok”

 ASSEMBLY

1. Select “Assembly” in the Module.
2. Clic on “Instance Part”… a. Select the part (Beam) b. Instance Type “Dependent” (mesh on part) c. Click “Ok”.