INTRODUCTION TO COMPUTATIONAL MECHANICS OF MATERIALS
Plane stress problem using ABAQUS package Linear statics + elastic-plastic analysis
Brief instruction
ABAQUS/CAE Standard: top menu, modules, trees for model and results.
Modules: Part, Property, Assembly, Step, Interaction, Load, Mesh, Job, Visualization, Sketch Solution of plane stress problem – linear statics:
1. Filling in Create Part window.
Name: plane stress elasticity, type: deformable, shape: solid, approximate size: 10.
2. Generation of geometry.
Module Part. Create lines: connected. Enter points, confirm using Done.
3. Definition of material – Edit Material window.
Name: elasticity. Mechanical → Elasticity → Elastic, type: isotropic, Young’s Modulus, Poisson’s Ratio.
4. Definition of section and section assignment.
Create Section window. Name: section, category: solid, type: homogenous.
After Continue tick plane stress/strain with thickness and enter thickness.
Find Section Assignment in model tree and choose appropriate section in the window.
5. Assignment of Part to Instance.
Select Assembly/Instances and choose part plane stress problem in Create Instance win- dow, mark instance type: independent.
6. Definition of steps, loading and boundary conditions.
Find Steps in model tree.
• Expand step called Initial and double click BCs to open Create Boundary Condi- tions window. Check category: mechanical, types for selected step: Symmetry/ An- tisymmetry/Encastre and go to Continue. Select the supported edge, confirm using Done button and in the next window called Edit Boundary Condition mark Encastre.
• Double click Steps in model tree and create next step called Step-1 (name can be changed). Choose the following options: insert new step after Initial, procedure type:
linear perturbation and go to Continue.
• Change Loads in new step, double click and open window for loading definition.
Choose appropriate step, category: mechanical, type: pressure and go to Continue button. Choose the loaded edge and confirm with Done button. In next window Edit Load mark distribution: uniform and insert magnitude of pressure (mind the unit).
7. Mesh generation.
Change module → Mesh. In toolbar click the following icons.
• In Mesh Controls: element shape – quad, technique – free, algorithm: medial axis.
Project ”The development of the didactic potential of Cracow University of Technology in the range of modern construction”
is co-financed by the European Union within the confines of the European Social Fund and realized under surveillance of Ministry of Science and Higher Education
1
• In Element Type window: element library – standard, family – plane stress, geometric order – linear or quadratic. In Quad options save defaults.
• In Global Seeds window: approximate global size – 0.21, tick curvature control, de- viation – 0.1. Confirm Apply.
• Choose Mesh/Instance and confirm generated discretization.
8. Computations.
Click Job in model tree and select Create Job. After creation of job – Data check can be (optionally) selected and Submit should be run in Job Manager. Results permit the user to switch to postprocessing.
9. Results.
In option Visualization all the results can be analyzed.
Solution of plane stress problem in plastic regime:
1. Copy of the model
Copy the model (in tree). Name: plane stress plasticity.
2. Redefinition of material – Edit Material window.
Rename: plasticity HMH. Mechanical → Plasticity → Plastic, yield strength, e.g.: 300e3, plastic strain: 0.
If hardening is defined, compute next points of hardening diagram and enter data in next rows to define a segment line, e.g. for linear hardening modulus equal to 2e6:
• in stress field, e.g.: 500e3,
• in strain field, e.g.: 0.1.
3. Redefinition of steps and loading.
Go to Steps in model tree.
• Delete Step-1.
• Double click Steps in model tree and recreate Step-1. Procedure type should now be defined as General and Static, General. After Continue in Incrementation op- tion Fixed should be indicated with maximum number of increments, e.g.: 100 and respective increment size: 0.01.
• Loading can be defined in the window, where category: mechanical, type: pressure are introduced. Select the loaded edge and confirm using Done button. In Edit Load window mark distribution: uniform and insert new magnitude for loading, for example:
100 000. A better option is to start the analysis with unit load, determine the load magnitude which will cause plastic yielding of the material, and define 2 steps: first to load the structure to just below the yield strength (this can be done in one increment since the analysis is linear) and second to enter and follow the plastic process in several increments.
4. New computations.
Click Job in model tree and select Create Job. After creation of new job (suggested name:
Compute plasticity) Data check can be (optionally) selected. Next Submit should be run in Job Manager.
5. Results.
Results permit the user to switch to postprocessing. In option Visualization all results can be observed: diagrams, displacements, plastic strain or equivalent stress distributions, etc.
Project ”The development of the didactic potential of Cracow University of Technology in the range of modern construction”
is co-financed by the European Union within the confines of the European Social Fund and realized under surveillance of Ministry of Science and Higher Education
2
