Limitations for Hot-Spot Stress (HSS) fatigue analysis
While the software allows local mesh refinement and stress visualization that may superficially resemble a hot-spot evaluation, the underlying CBFEM formulation does not satisfy the methodological requirements of the structural stress approach.
Design Philosophy of CBFEM and Its Implications
The Component-Based Finite Element Method (CBFEM) implemented in IDEA StatiCa was developed for a specific purpose: plastic ULS verification of joints in accordance with EN 1993-1-8. The following modeling choices reflect that scope:
| Feature | Implementation in CBFEM | Implication for Hot-Spot Stress |
| Mesh density | Coarse-to-medium shell mesh, optimized for force redistribution | Insufficient resolution for stress recovery at the weld toe |
| Material model | Elasto-plastic with a 5% strain limit | Deliberately smears stress peaks at geometric notches |
| Weld representation | Multi-Point Constraint (MPC) coupling between plates | No physical weld toe geometry exists in the model |
| Plate connectivity | Plates terminate at the connection face; midlines fully coupled | The geometric transition that drives the hot-spot stress is not represented |
| Stress output | Equivalent (von Mises) stress on plate elements | Not the principal stress component normal to the weld toe required by HSS |
Each of these is appropriate for component-level ULS design but incompatible with the structural stress methodology, which presupposes that the geometric stress concentration at the weld toe is explicitly captured by the FE model.
Methodological Requirements of the Hot-Spot Stress Approach
For reference, EN 1993-1-9 Annex B and the IIW recommendations require:
- Mesh size of
t × tat the hot-spot location, with appropriate refining within the extrapolation zone. - Surface stress recovery at the reference points 0.4·t and 1.0·t from the weld toe (for type "a" hot-spots).
- A geometrically defined weld toe — either modeled explicitly with throat and toe, or located at the theoretical toe position on the parent plate surface.
- Linear (or quadratic) extrapolation of the principal stress oriented within ±60° of the normal to the weld toe.
None of these conditions is intrinsically satisfied by the IDEA StatiCa Connection model.
What Is Partially Feasible in IDEA StatiCa
In the interest of transparency, the following operations are technically possible, though they do not constitute a compliant HSS assessment:
Local Mesh Refinement
- Element size on individual plates can be controlled via Mesh Setup → element size.
- Refinement down to ~2–4 mm in critical zones is achievable.
- For a representative plate thickness of t = 15-25 mm, this still falls short of the four to six elements resolution required for reliable extrapolation.
Stress Visualization
- Equivalent stress (σ_eq, von Mises) is available on the plate surface.
- Stress values at approximate positions corresponding to 0.4·t and 1.0·t can be read manually using the cursor or the section cut tool.
- However, von Mises is not the correct stress measure for HSS extrapolation; the principal stress component normal to the weld toe is required.
What Does Not Work
- Weld geometry: Welds are represented as MPC constraints with force/stress recovery on a virtual throat. The plate terminates at the connection face, so no weld toe geometry exists to extrapolate toward.
- Node placement at extrapolation points: The mesher does not permit explicit node placement at 0.4·t and 1.0·t. Stresses are recovered at integration points and extrapolated to nodes at locations dictated by the mesh generator.
- Post-processing: There is no built-in linear/quadratic extrapolation function, no principal-stress-orientation check relative to the weld toe, and no fatigue output module for either the structural stress or notch stress approaches.
Clarification on the Non-Physical Weld Representation
It is important for users to understand that the butt weld option in IDEA StatiCa is a non-physical modeling abstraction. The connected plates are coupled through constraint equations along their midlines, and the weld itself has no discrete geometric representation in the FE mesh. Without a physically modeled weld toe — and without verification against a refined solid or shell submodel — no definitive claim regarding the validity of an HSS reading taken from this model can be made.
Recommended Workflow for Fatigue-Critical Connections
IDEA StatiCa Connection performs ULS design checks in accordance with EN 1993-1-8. Fatigue is not a standard output. For connections governed by fatigue, the following workflow is recommended:
- Use IDEA StatiCa Connection to:
- Validate the ULS capacity of the joint.
- Extract internal forces and nominal stress states on the relevant plates and welds far from the discontinuity region.
- Perform the fatigue verification externally using:
- The nominal stress approach per EN 1993-1-9 with the appropriate detail category, where the geometry corresponds to a tabulated detail.
- For non-standard details or where the nominal approach is not applicable (complex geometry, attachments without a tabulated category, very thick plates):
- Use a dedicated FEA package (e.g., Abaqus or ANSYS) to build a shell or solid submodel that meets the IIW mesh and weld-modeling requirements.
- Apply the structural (hot-spot) stress or effective notch stress approach as appropriate.
- Couple the submodel to the IDEA results through equivalent boundary forces or imposed displacements.
For fatigue-critical or non-standard details, fatigue verification should be performed externally using either the nominal stress approach or a dedicated FE submodel built for the structural/-notch stress methodology.