Structural and Thermal Analyses

4.1  Static Structural: Setup

Boundary conditions define the rigid-body constraint and load application. The constraint must match the physical installation — over-constraining gives artificially low deflection and stress; under-constraining causes rigid-body motion and solver failure.

Support types

• Fixed support: all degrees of freedom at the selected face are zero. Use at bolted connections when the bolt interface is substantially stiffer than the structure.
• Frictionless support: normal displacement constrained, lateral free. Use at symmetry planes and at surfaces resting on a flat rigid fixture.
• Elastic support: spring stiffness between surface and ground. Use when the supporting structure has a known compliance.
• Displacement: prescribes specific displacement values at a surface. Use for imposed deformation boundary conditions.

Load types

• Acceleration: applies a body force proportional to component mass. The standard input for g-load qualification (transportation, seismic, shock).
• Force / pressure: direct load at known magnitude and direction.
• Thermal condition: imported temperature field from a linked thermal analysis. Drives CTE expansion.

Contact definitions

• Bonded: no separation or sliding. Default for soldered, adhesively bonded, or press-fit interfaces.
• Frictional: Coulomb friction model. Use when slip and friction force affect the structural result.
• No separation: surfaces cannot pull apart but can slide freely. Use at sliding interfaces that cannot separate under the applied load.

Verify setup before solving: insert a Reaction Force probe at the support (Solution → Insert → Probe → Force Reaction). The sum of reaction forces must equal the sum of applied forces. A significant imbalance means the model is incorrectly constrained.

4.2  Static Structural: Results

Von Mises (equivalent) stress

The standard yield criterion for ductile metals (steel, aluminum, copper). Compare directly to yield strength. Safety factor = yield strength / Von Mises stress. Use as the primary result for metals.

Maximum principal stress

The largest tensile stress at a point. Use for brittle materials (FR4 laminate, ceramic, glass) and for crack growth assessment. FR4 fails in tension on the outer fiber — maximum principal stress is the relevant criterion.

Total deformation

Displacement magnitude. Use to verify that deflections do not cause secondary failures: connector disengagement, interference with adjacent components, or board-level curvature exceeding component attachment limits.

Mesh singularities

A perfectly sharp re-entrant corner in a finite element model produces stress that grows without bound as the mesh is refined. This is a modeling artifact, not a physical stress. Distinguish a singularity from a real stress concentration:

• At a fillet or radius: stress converges to a finite value as mesh refines. This is physically real — report it.
• At a perfectly sharp internal corner: stress increases without converging as mesh refines. Replace the corner with the minimum physical radius from manufacturing tolerance, then re-run.

4.3  Modal Analysis

Ansys Learning Hub: Mechanical Beyond the Basics ↗ · 7 hr · E-learning

Modal analysis computes the natural frequencies and mode shapes of the structure. It is always run before random vibration analysis — random vibration requires modal results as its upstream input.

Setup: apply the same structural supports as the static analysis. No loads are required (modal is a free-vibration problem — the solver finds frequencies at which the structure vibrates naturally given its mass and stiffness distribution). Set the number of modes to extract to cover at least 1.5× the highest frequency of interest in the subsequent random vibration analysis.

The solver computes natural frequencies ω and mode shapes {φ} from: [K]{φ} = ω²[M]{φ}. Mode shapes are unit-normalized — the reported displacement magnitude has no physical meaning. Only the shape matters. Visualize each mode to identify which structural elements participate: a mode dominated by board flexure behaves differently under vibration than a mode dominated by component rocking.

Free-free modal (no supports): if supports are removed, the first six modes will be rigid-body modes at near-zero frequency. These are correct but not useful. The first flexible mode is the lowest frequency above the rigid-body modes.

4.4  Random Vibration (RSD/PSD)

Random vibration analysis applies a Power Spectral Density (PSD) spectrum to the modal results to compute the statistical stress and displacement response in a broadband vibration environment.

Setup

Link the Modal analysis upstream. Define the PSD spectrum: acceleration (G²/Hz) vs. frequency, obtained from the qualification test specification or field measurement data. Run the analysis in each of the three principal directions (X, Y, Z) separately. ANSYS recommends extracting enough modes to cover 1.5× the maximum frequency in the PSD excitation.^[1]

Result interpretation

All results (stress, displacement) are reported as 1-sigma (one standard deviation) values — meaning 68.3% of the time the response will be less than that value. You can scale the result by 2 to get 2-sigma values (95.45% probability) or by 3 to get 3-sigma values (99.73% probability) via the Scale Factor property in the Solution branch.^[1]

Random vibration results are statistical — they do not represent any single point in time. The 3-sigma stress cannot be compared to yield strength as a failure criterion in the same way static stress can. For qualification, compare to the fatigue allowable or the test-verified acceptance threshold specified in the applicable standard.

4.5  Steady-State Thermal and CTE-Driven Stress

Ansys Learning Hub: Mechanical Advanced Material Modeling ↗ · 8 hr · E-learning

The thermal-structural workflow links two Workbench systems: a Steady-State Thermal analysis that computes the temperature distribution, and a Static Structural analysis that imports the temperature field and computes the resulting thermal expansion stress.

Steady-State Thermal setup

Inputs: thermal conductivity for all materials, power dissipation at each heat source (component power), and convection coefficients or convection boundary conditions at surfaces exposed to air. The output is a nodal temperature distribution.

Thermal-structural link

In the Static Structural analysis, insert a Thermal Condition load (Solution → Insert → Thermal Condition). This maps the temperature field from the thermal analysis onto the structural mesh node-by-node. Where the structural and thermal meshes differ (separate systems), ANSYS interpolates the temperatures. Verify the transfer: plot temperature in the structural model before solving. An incorrect transfer appears as uniform ambient temperature everywhere — if the temperature field looks constant, the link is broken.

Stress-free reference temperature

The structural model computes thermal expansion relative to a reference temperature — the temperature at which the assembly is stress-free. For soldered assemblies, this is approximately the reflow temperature (~260°C for lead-free solder), not room temperature. An incorrect reference temperature produces incorrect CTE stress magnitude and direction.

4.6  Plastic Deformation

Standard linear analysis assumes stress is proportional to strain and that the material returns to its original shape when the load is removed. When stress exceeds the yield strength, neither assumption holds. Plastic analysis uses a nonlinear material model to follow the stress-strain curve through yield.

Material model

Two common options in ANSYS Engineering Data:

• Bilinear isotropic hardening (BISO): two-slope approximation. Requires elastic modulus, yield strength, and tangent modulus. Simple and computationally efficient. Appropriate when the full stress-strain curve is not available.
• Multilinear isotropic hardening (MISO): full stress-strain curve entered as a table. More accurate for large plastic strains. Requires material testing data or certified datasheet values.

Solver and convergence

Plastic analysis uses Newton-Raphson iteration at each load step. If it does not converge: reduce the load step increment first (split the load into more steps). Do not change the material model or mesh as a first response to convergence failure. Convergence failure at a particular load level indicates that the material is being pushed past a steep region of the stress-strain curve — smaller steps resolve this.

If full stress-strain data is not available: run the analysis as linear-elastic and compare peak Von Mises stress to yield strength. Regions above yield in the elastic model will yield — the elastic result does not give the post-yield state, but it identifies which locations require attention.

4.7  Solver Non-Convergence and Solution Verification

Two distinct concepts are often conflated: solver convergence (did the Newton-Raphson algorithm reach equilibrium?) and mesh convergence (is the mesh fine enough that the result is independent of it?). Both must be addressed before trusting a result.

Reading the convergence plot

Open Solution Information (the wrench icon under the Solution branch) and select the Force Convergence tab. The plot shows the normalized force residual at each iteration. A converged substep shows the residual falling monotonically below the convergence criterion (default 0.5% of the reference force). Divergence looks like a residual that oscillates, plateaus, or increases across iterations.

The residual does not need to drop to zero. It needs to drop below the criterion. If the analysis terminates with "Solver failed to converge," the Solution Information file shows the last-attempted substep and which Newton-Raphson iteration it stalled at. Start reading there.

Common causes and remedies

Contact instability

The most common cause of non-convergence in assemblies. Contact status changes between open and closed across iterations (chattering), preventing the global stiffness from settling. Indicators: the force residual oscillates without decreasing; the Solution Information shows "contact status changed" messages.

• Set initial contact state to Adjust to Touch: eliminates initial penetration that drives the first iteration into instability.
• Reduce the time step: smaller substeps prevent large contact status swings between iterations.
• Enable Contact Stabilization (contact pair settings): adds a damping term to contact that stabilizes chattering. Remove it after confirming convergence — it is not physically real.
• Check pinball radius: if the gap between faces is larger than the pinball region, contact is never detected. Increase if surfaces are near but not touching.

Rigid body motion

If the model has a free-floating body with no constraints or active contact, the solver produces a near-zero pivot in the stiffness matrix and terminates. The Solution Information shows "a Pivot check has failed" or large displacement warnings.

• Enable Weak Springs (Analysis Settings → Solver Controls): ANSYS adds tiny springs to all unconstrained bodies to prevent rigid-body motion. These springs should not carry significant reaction force — check this after convergence. If they do, the model is under-constrained and the springs are masking a setup error.
• Review contact definitions: a disconnected body usually has a missing bonded contact pair. Use the Contact Tool (Connections → Contact Tool) to check which pairs are open.

Large deformation not enabled

For problems where deflections are comparable to the part dimensions, the small-strain formulation loses accuracy because it does not update the stiffness matrix for the deformed geometry. Symptoms: diverges at a load level where deflections are clearly large, or the result looks wrong with excessive deflections.

Enable: Analysis Settings → Large Deflection = On. This triggers an updated Lagrangian formulation that reformulates the stiffness matrix at each substep. The solve becomes slower and may require more substeps, but the physics is correct.

Bisection and load step control

When nonlinear analyses fail to converge at a substep, ANSYS automatically bisects — halves the load step and retries. The Solution Information shows "Bisection occurred." This is normal for the solver to recover from difficult load increments. If it bisects more than 5 times in succession, the problem is structural: the material or contact state at that load level is genuinely difficult. Review the geometry and material inputs at that load level.

To give the solver more room to work: Analysis Settings → Number of Substeps → set minimum to 10 and maximum to 200. The solver will use what it needs.

Mesh convergence study

Solver convergence says the Newton-Raphson algorithm found an equilibrium. It says nothing about whether that equilibrium is the correct physical answer — which depends on whether the mesh is fine enough to resolve the gradient.

Method: run the same analysis at two or three mesh densities. In the critical region (where the peak stress or temperature is located), refine the element size by 2— between each run. Extract the peak value at the same location across all runs and compare.

• Converging result: peak value changes by less than ~5% between the two finest meshes. The mesh is adequate. Report the finest-mesh result.
• Still changing significantly: refine further. The gradient is not resolved.
• Increasing without bound as elements get smaller: mesh singularity. A perfectly sharp re-entrant corner (zero radius) produces a stress that is theoretically infinite. The finite element solution converges to infinity with refinement — this is mathematically correct but physically wrong. Fix: add a fillet in SpaceClaim. Real parts have a minimum radius determined by machining or manufacturing process. Use that radius.