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.
4.
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