Abaqus Tutorial: A Complete Beginner's Guide to Abaqus CAE

What is Abaqus?

Abaqus is a general-purpose FEA software suite — one of the most powerful and widely used in the world — for solving highly nonlinear structural, thermal, and coupled problems in aerospace, automotive, biomedical, and civil engineering.

Developed by Hibbitt, Karlsson & Sorensen, Inc. in 1978 and now owned by Dassault Systèmes Simulia, Abaqus is particularly renowned for its advanced nonlinear capabilities — complex material models, contact algorithms, and large deformation analysis that goes beyond what many general-purpose FEA tools can handle robustly.

Abaqus components

The Abaqus suite comprises several software components:

The 9 Abaqus CAE modules

Abaqus CAE is organised into 9 functional modules accessible from the Module drop-down at the top of the interface. Each module focuses on a specific step of the FEA workflow:

1. Part module

Create the geometry of each component in your model. You can sketch 2D profiles and extrude/revolve/sweep them into 3D solids, or import geometry from CAD files (IGES, STEP, CATIA, SolidWorks, etc.). Each part is independent — they are combined in the Assembly module.

2. Property module

Define material properties (elastic modulus, Poisson's ratio, density, plasticity curves, failure criteria) and assign sections (solid, shell, beam, truss) to each part. This module contains Abaqus's extensive material library — including metals, composites, elastomers, foams, and concrete.

3. Assembly module

Create instances of your parts and position them relative to each other to build the full assembly. Constraints (contact pairs, tie constraints, rigid body connections) are defined here in conjunction with the Interaction module.

4. Step module

Define the analysis steps — Static General, Static Riks (post-buckling), Dynamic Implicit, Dynamic Explicit, Frequency (modal), Heat Transfer, Coupled Temperature-Displacement, and more. Also configure output requests (field outputs to the .odb, history outputs for time-history data).

5. Interaction module

Define contact between surfaces (surface-to-surface, general contact), constraints (tie, rigid body, coupling, MPC), and connectors (springs, dashpots, actuators). Getting contact definitions right is often the most challenging part of nonlinear FEA models.

6. Load module

Apply boundary conditions (displacement, fixed support, symmetry) and loads (concentrated force, pressure, body force, thermal load, predefined fields). Loads can be ramped, stepped, or defined using amplitude curves for time-varying analysis.

7. Mesh module

Seed edges with element density, select element types (C3D8R, C3D10, S4R, B31, etc.), and generate the mesh. Mesh controls allow structured (hex-dominant) or free (tet) meshing. Verifying mesh quality — aspect ratio, warp factor, distortion — is a critical step before running.

8. Job module

Create and submit analysis jobs. Monitor convergence in the Abaqus Job Monitor (increments, iterations, warnings). Jobs can be submitted locally or to a cluster via queue scripts. The .inp file generated here can be edited manually for advanced configuration.

9. Visualisation module (Abaqus Viewer)

Post-process results from the .odb output database: plot contours (S, Mises, U, PE, PEEQ), deformed shapes, X-Y histories, generate animations, and extract tabular data. Free-body cuts, path plots along lines, and surface-averaged results are all available.

Step-by-step tutorial: cantilever beam under point load

This tutorial walks through a simple 3D cantilever beam — 200 mm × 20 mm × 10 mm, steel, with a 500 N downward point load at the free end. Target: predict maximum deflection and Von Mises stress.

Step 1: Create the Part

Open Abaqus CAE. Module → Part. Click "Create Part". Name: Beam. Type: 3D Deformable Solid. Shape: Solid/Extrusion. Click Continue. Sketch a 200 mm × 20 mm rectangle. Extrude 10 mm depth. Click Done.

Step 2: Define the Material and Section

Module → Property. Create Material: Name "Steel". Mechanical → Elasticity → Elastic: E = 210,000 MPa, ν = 0.3. Density = 7.85e-9 t/mm³. Create Section → Solid, Homogeneous, Material = Steel. Assign Section to the beam part.

Step 3: Create the Assembly

Module → Assembly. Create Instance → Independent (mesh on instance). Your beam part appears in the viewport. No position adjustments needed for a single-part model.

Step 4: Define the Step

Module → Step. Create Step → Static, General. Name: "Loading". Time Period = 1.0. Incrementation: Initial = 0.1, Min = 1e-5, Max = 0.1. Field Output: S, U, RF, E (add PEEQ if plasticity is needed).

Step 5: Apply Boundary Conditions and Load

Module → Load. Create Boundary Condition → Displacement/Rotation → select the clamped face (x=0 face): fix U1=U2=U3=UR1=UR2=UR3=0. Create Load → Concentrated Force → select the node at the free-end centre: CF2 = -500 N (negative Y direction).

Step 6: Mesh

Module → Mesh. Seed Part Instance → global seed = 5 mm. Assign Element Type → C3D8R (8-node linear brick, reduced integration — the workhorse element for most structural problems). Mesh Part Instance. Verify mesh quality (green elements = acceptable).

Step 7: Submit the Job and Monitor

Module → Job. Create Job → Name: "Beam_Analysis". Submit. Open Job Monitor to watch convergence. Typical run time for this model: under 5 seconds on any modern workstation.

Step 8: Visualise Results

When complete, click Results. Module → Visualisation. Plot Contours → S, Mises to view Von Mises stress distribution. Plot Contours → U, U2 for vertical deflection. The analytical solution for maximum deflection of a cantilever is δ = PL³/(3EI) — compare this to your FEA result to validate the simulation.

For a 200 × 20 × 10 mm steel cantilever: I = bh³/12 = 20×10³/12 = 1,666.7 mm⁴. δ_analytical = (500 × 200³)/(3 × 210,000 × 1,666.7) = 1.905 mm. Your Abaqus result should match within <1% with this mesh density.

Python automation in Abaqus

Every action you perform in Abaqus CAE is recorded as a Python command in the replay file (abaqus.rpy). Use Plug-ins → Macros → Start Recording to record a sequence of actions, then inspect the generated Python commands. This is the fastest way to learn the Abaqus Python API.

Once familiar, you can write scripts to parametrically modify models, run hundreds of design iterations, and extract and process results automatically — without touching the GUI. Run scripts from File → Run Script, or pass them to the Abaqus command line: abaqus cae script=my_script.py.

Frequently asked questions