Load Case vs. Load Step: Understanding Solver Architecture and Non-Linearity
Executive Summary
In Finite Element Analysis (FEA), the terminology surrounding load application often leads to confusion—particularly when transitioning between different commercial solvers such as MSC Nastran, Abaqus, Ansys, or Altair OptiStruct. Keywords like Load Case (or SUBCASE) and Load Step (or *STEP) are sometimes used interchangeably in casual engineering conversations, yet they represent two fundamentally different solver architectures. Confusing a Load Case with a Load Step is not merely a semantic error; it reflects a deeper misunderstanding of whether a structural system obeys linear superposition or follows a path-dependent non-linear history.
1. Load Cases (Nastran SUBCASE): The Power of Linear Superposition
A Load Case (historically rooted in linear codes like MSC Nastran or Ansys linear static modules) represents an independent loading condition solved on a fixed, unyielding global stiffness matrix [K].
In a purely linear static analysis, the fundamental governing equation simplifies to:
Because the stiffness matrix [K] remains strictly constant regardless of the applied force or displacement magnitude, commercial solvers factor [K] into upper and lower triangular matrices (LU decomposition) only once. Subsequently, the solver can process dozens or hundreds of different right-hand side force vectors {F1}, {F2}, …, {Fn} using fast back-substitution.
Didactic Matrix Inversion Note: In practical industrial FEA, computing the explicit inverse [K]-1 is computationally prohibitive and avoided via direct factorization methods (LU decomposition). However, for educational clarity, Appendix B of my book, Computational Structural Engineering, presents a simplified hand-calculation example where [K] is explicitly inverted to illustrate the exact mathematical mechanics behind {u} = [K]-1 · {F}.
- Independence: Load Case 2 does not inherit stress, strain, or displacement from Load Case 1. Each
SUBCASEis completely independent. - Computational Efficiency: Solving additional load cases requires minimal extra CPU time since matrix inversion/decomposition is performed only once.
- Applicability: Linear static stress analysis, normal mode extraction (eigenvalue analysis), classical linear buckling (eigenvalue buckling), and fatigue duty cycle superpositions.
2. Load Steps (Abaqus *STEP): Path-Dependent Sequential History
In contrast, a Load Step (pioneered by non-linear engines like Abaqus) represents a chronological sequence in time or pseudotime. In a step-based architecture, the final state of Step N serves as the initial boundary condition, stress state, and geometry for Step N+1.
Whenever non-linearities are introduced—such as large deformations (geometric non-linearity), material plasticity, or status-changing surface contact—the global stiffness matrix becomes a function of displacement and load history: [K(u)].
Linear Load Cases in Abaqus (*STEP, PERTURBATION)
It is important to note that step-based solvers like Abaqus can also execute traditional linear load cases when required. By using the syntax:
Abaqus treats the step as a purely linear perturbation around a specific base state. In this mode, multiple load cases can be evaluated efficiently on a frozen stiffness matrix, mimicking the behavior of Nastran SUBCASE definitions while allowing engineers to analyze linear responses around non-linearly pre-stressed assemblies.
3. Feature Comparison: Load Step vs. Load Case
The following feature matrix highlights the operational capabilities and limitations of Load Steps (e.g., standard non-linear Abaqus *STEP) versus Load Cases (e.g., Nastran SUBCASE or Abaqus PERTURBATION steps):
| Feature | Load Step (Abaqus *STEP) | Load Case (Nastran SUBCASE) |
|---|---|---|
| Stiffness Matrix Can Change | YES | NO |
| Fast Solution | NO | YES |
| Large Deflection (NLGEOM) | YES | NO |
| Contact Mechanics | YES | NO |
| Material Plasticity | YES | NO |
| Multiple Load Conditions | NO | YES |
| Buckling Analysis | NO (*) | YES |
| Normal Mode Analysis | NO | YES |
| Linear Analysis | YES (**) | YES |
| Non-Linear Analysis | YES | NO |
(*) Note: Post Buckling Analysis (e.g., Riks arc-length method) can be performed instead in a non-linear step.
(**) Note: A Linear Analysis can be performed as Non Linear inside a step, but it would be a waste of time and calculation resources.
4. Practical Engineering Guidelines
When structuring your finite element models, choosing between a load case or load step strategy depends entirely on physical assumptions:
- Use Load Cases when: You are evaluating structural integrity across multiple independent operating environments (e.g., g-loads, wind directions, thermal load envelopes) where deformations remain small, materials stay elastic, and boundary conditions do not change.
- Use Load Steps when: The physical process is sequential (e.g., bolt pre-tensioning in Step 1, followed by working pressure in Step 2), or when capturing surface interactions, large rotations, or permanent plastic deformation.
- Linear Perturbation Steps: Modern solvers allow hybrid approaches. For instance, a non-linear load step can establish a pre-stressed base state (including contact engagement and bolt pre-load), followed by a linear perturbation step (
*STEP, PERTURBATION) to extract natural frequencies or perform linear modal dynamic calculations around that deformed equilibrium state.
5. Conclusion
Understanding whether your simulation requires independent Load Cases or sequential Load Steps is critical for choosing the right solver, avoiding numerical errors, and preventing wasted computational resources.
Appendix B of the book Computational Structural Engineering explores the mathematical formulation of element matrices and global stiffness matrix assembly and solver algorithms, detailing step-by-step matrix operations up tp the solution for linear structural systems.
