it describes analysis of plane truss using abaqus and also the introduction to analysis window

1. FE Lab – CE5131
Introduction to Abaqus

2. Introduction
 Abaqus is a collection of engineering simulation problems, based on the finite element method.
 Abaqus can solve relatively simple linear analyses to the most challenging nonlinear simulations.
 Extensive library of elements
 Extensive list of material models
 Apart from structural (stress/displacement) problems:
 Heat transfer,
 Mass diffusion,
 Thermal management of electrical components(coupled thermal-electrical),
 Acoustics,
 Soil mechanics (coupled pore fluid-stress analysis)
 piezoelectric analysis

3. Stages of
Analysis
 Preprocessing
 Define the model of the
physical problem
 Create and Abaqus input
file
 Simulation
 Solves the numerical
problem defined in the
model
 Postprocessing
 Evaluation of results.

5. Title bar Menu bar Tool bar Context bar
Model tress/
Results tree
Toolbox
area
Viewport
Message area or
Command line interface area

6. Consistent
units
• Abaqus has no built-in system of units.
• Do not include unit names or labels while entering data.
• All input data must be specified in consistent units.

7. Components of an Abaqus analysis model
Discretized geometry
Element section properties
Material data
Loads and boundary conditions
Analysis type
Output requests

8. Product features and Limitations – Learning Edition 2022
The Abaqus Learning Edition consists of Abaqus/Standard, Abaqus/Explicit, and Abaqus/CAE.
Full HTML documentation is included.
The maximum model size is limited to 1000 nodes for structural analysis and postprocessing.
Features requiring compilers are not available (user subroutines).
Parallel execution is not available.
Add-on products are not available

9. Example 1 – Truss
Analysis
 Determine the nodal deflections
and stresses for the truss system
shown.
 It is given that Young’s modulus
(E) =200 Gpa, Poisson’s ratio =
0.3, and cross-section area (A) =
3250 mm2
 Left end is constrained and right
end is supported on a roller.
 We will perform a simulation in
Abaqus/Standard to determine
structure’s deflection and peak
stress in its members when a
load of 400 kN is applied @ 3
nodes as shown in the figure.
Simply supported Plane truss

10. Example 1 – Truss Analysis
Start → Abaqus CAE → Create Model Database with Standard/Explicit Model
File → Set Working Directory → Select the desired directory → OK
File → Save As → Save Truss_analysis.cae file in Work Directory
Module: Part ==> Part → Create → Select 2D Planar, Deformable, Wire → Continue (It opens the
Sketch module)
 Module: Sketch ==> Create Isolated Points → Enter Coordinates (X, Y): (0, 0), (2000, 3500),
(4000, 0), (6000, 3500), (8000, 0), (10000, 3500), (12000, 0) (Right click → Cancel Procedure)
View → Auto-Fit
Create Lines: Connected → Select two points (1 and 2 shown in figure) to create a line (Right click
→ Cancel Procedure) → Repeat this step for creating all the lines → Done

11. Example 1 – Truss Analysis
Module: Property ==> Material → Create → Name: Material-1, Mechanical, Elasticity, Elastic →
set Young's modulus = 200e3, Poisson's ratio = 0.3 → OK
Section → Create → Name: Section-1, Truss → Continue → set Material: Material-1, Cross-
sectional area: 3250
Assign Section → select all elements by dragging mouse → Done → Section-1 → OK → Done
Module: Assembly ==> Instance → Create → Create instances from: Parts → Part-1 → Dependent
(mesh on part) → OK
Module: Step ==> Step → Create → Name: Step-1, Initial, Static, General → Continue → accept
default settings → OK

12. Example 1 – Truss Analysis
Module: Load ==> BC → Create → Name: BC-1, Step: Initial, Mechanical, Displacement/Rotation
→ Continue → select point 1 → Done → select U1 and U2 → OK
BC → Create → Name: BC-2, Step: Initial, Mechanical, Displacement/Rotation → Continue →
select point 7 → Done → select U2 → OK
Load → Create → Name: Load-1, Step: Step-1, Mechanical, Concentrated Force → Continue →
select points 2, 4 and 6 → Done → set CF2: -400000 → OK
Module: Mesh ==> Set Model: Model-1, Object → Part: Part-1
Seed → Edges → select entire truss by dragging mouse → Done → Method: By number, Bias:
None, Sizing Controls, Number of Elements: 1 → press Enter → Done

13. Example 1 – Truss Analysis
Mesh → Element Type → select entire truss by dragging mouse → Done → Element Library:
Standard, Geometric Order: Linear: Family: Truss → OK → Done
Mesh → Part → OK to mesh the part Instance: Yes
Module: Job ==> Job → Create → Name: Job-1, Model: Model-1 → Continue → Job Type: Full
analysis, Run Mode: Background, Submit Time: Immediately → OK
Job → Submit → Job-1
Job → Manager → Results (transfers to Visualization Module)
Module: Visualization ==> View → Graphics Options → Viewport Background = Solid→ Color →
White (click on black tile to change background color)

14. Example 1 – Truss Analysis
Options → Common → Labels → select 'Show element labels: Black' and 'Show node labels: Red’
→ OK
Plot → Undeformed Shape
Plot → Deformed Shape
Plot → Contours → On Deformed Shape
Result → Options → unselect “Average element output at nodes”
Result → Field Output → Component: S11 → OK
Ctrl-C → Copies graphics window to clipboard → Paste in MS Word, etc.
Report → Field Output → Variable → Position: Unique Nodal → select U: Spatial Displacements →
Apply → Unselect U

15. Example 1 – Truss Analysis
Report → Field Output → Variable → Position: Centroid → select S: Stress Components → Click on
‘>’ and unselect all stresses except S11 → Apply → Cancel
Open file ‘Abaqus.rpt’ and cut and paste desired results into MS Word
File → Save → enter desired file name (Abaqus will append .cae)
File → Exit