Phase 7

Multi-Physics and Result Communication

The preceding phases built each analysis tool independently. This phase connects them. A Workbench project that links Maxwell losses to Icepak heat sources and Mechanical structural stress represents the complete simulation chain for a power electronics assembly. The phase closes with the minimum requirements for presenting simulation results at a design review.

7.1  Workbench Multi-Physics Linking

Ansys Learning Hub: Electrothermal Management (ETM) using Maxwell and Icepak ↗ · 2 hr · E-learning  ·  IcepakFEA ↗ · 8 hr

Analysis systems in Workbench are linked by connecting their cells in the Project Schematic. The connection type determines what information transfers.

Geometry link
Connects the Geometry cell of one system to the Geometry cell of another. Both systems share the same SpaceClaim body. A geometry update in SpaceClaim propagates to all linked systems simultaneously. This is the correct setup for any analysis sharing the same physical part.
Mesh link
Connects the Mesh cell between two systems. Both systems share the same nodal mesh. Used when Steady-State Thermal and Static Structural should solve on identical nodes to eliminate interpolation error in the temperature transfer.
Solution link
Passes a result from one system's Solution cell as an input to another system's Setup cell. Examples: Maxwell → Icepak (loss map), Steady-State Thermal → Static Structural (temperature field).

Maxwell to Icepak link

Connect the Maxwell Solution cell to the Icepak Setup cell. The link transfers the geometry, excitation definition, and the volumetric loss map (W/m³). Icepak uses the loss map as the distributed heat source for the conductor and core bodies. The connection updates automatically when Maxwell is re-solved — but does not trigger Icepak to re-solve. The Icepak system shows "Needs Update" and must be re-solved explicitly. For the 20 kHz transformer worked in section 6.5, the full chain is Maxwell (loss map at switching frequency) → Icepak (thermal solve with distributed heat source) → Mechanical Structural (CTE stress driven by the Icepak temperature field) — three solvers, one SpaceClaim geometry source, updated in sequence.

7.2  Design Change Propagation

A geometry change in SpaceClaim propagates through the analysis chain in a defined order. Each system downstream of the change must be updated before its results are valid.

Typical propagation order for an electromagnetic-thermal chain:

  1. SpaceClaim geometry update
  2. Maxwell geometry import (Needs Update)
  3. Maxwell solve (Needs Update)
  4. Icepak geometry import (Needs Update via loss link)
  5. Icepak mesh (Needs Update if geometry changed significantly)
  6. Icepak solve (Needs Update)
  7. Mechanical Structural temperature import (Needs Update if linked to Icepak)
  8. Mechanical solve (Needs Update)

The rule: update from the topmost stale cell down. Never update a downstream cell without updating all cells above it in the chain. Doing so produces results on stale upstream inputs — the "Needs Update" indicator on the downstream cell will clear, but the results are not current.

Validation after a design change

After propagating an update, verify three things before reporting results:

  • The geometry change is visible in the downstream model — inspect the viewer to confirm the change propagated correctly.
  • The mesh quality is still adequate — check metrics after re-mesh. A geometry change can introduce new sliver faces or degrade quality in the modified region.
  • Boundary conditions still apply to the correct faces — a geometry change can delete the face that a fixed support, heat source, or excitation was applied to. Missing boundary conditions do not always produce solver errors; they may produce silently wrong results.
Example — inverter assembly: propagating a switching frequency change through the full chain

An inverter initially designed at 15 kHz. A design change increases the switching frequency to 20 kHz to reduce filter inductor size. The full analysis chain: Maxwell → Icepak → Mechanical Structural.

  1. Maxwell re-solve at 20 kHz: transformer winding AC losses increase from 0.62 W to 0.78 W (+26% — smaller skin depth at 20 kHz concentrates current more). Core losses increase from 0.41 W to 0.54 W (Pcore ∝ f1.25 for N87). Total transformer loss: 1.32 W vs 1.03 W at 15 kHz. Maxwell shows “Up to Date.”
  2. Icepak — Needs Update: the Maxwell → Icepak loss link marks Icepak as needing update. No geometry change — only heat source values changed. The transformer mesh does not need regeneration; only the heat source magnitudes update when Icepak is re-solved.
  3. Icepak re-solve: transformer body T-rise increases by 9°C due to the additional 0.29 W. Peak transformer winding temperature: 88°C → 97°C. FET temperatures are unchanged (their losses did not change with frequency).
  4. Mechanical — Needs Update: higher transformer temperature increases CTE-driven solder joint stress at the transformer mount. Re-solve: stress at the transformer solder joints increases by 4 MPa.

Post-change validation:

  • Boundary conditions still target valid geometry: no geometry change occurred, so all BCs remain attached to the correct faces.
  • Mesh quality: unchanged (no geometry modification).
  • Decision: 9°C transformer temperature rise is acceptable (97°C vs 105°C limit). 4 MPa solder stress increase is within margin. Frequency change is approved.

7.3  Result Communication and Documentation

A simulation result presented at a design review must carry enough context to be interpretable and checkable. A stress contour plot without context cannot be evaluated — it is not possible to determine whether it represents a safe design without knowing what assumptions produced it. A statement such as “Tjunction = 97°C” at a design review is not interpretable without stating: which FET, at what power level, at what ambient temperature, with what airflow, and whether the TIM conductivity was measured or assumed.

Minimum required context for any simulation result

  • ANSYS version — which solver version produced the result.
  • Analysis type — e.g., "Steady-state thermal with JEDEC compact component models; forced convection not modeled."
  • Material assumptions — any non-default or estimated material properties, e.g., "FR4 through-thickness conductivity assumed 0.3 W/m·K."
  • Boundary condition summary — how constrained, where loads applied, what convection coefficient or CFD boundary was used.
  • Mesh quality — worst-case skewness and orthogonal quality; or, if mesh convergence was verified, state the refinement ratio and the change in the result quantity.
  • Key assumptions — any simplification of reality: no radiation, no contact resistance, uniform power, symmetric model, etc.
  • Known limitations — what the model does not capture that could affect the conclusion.

What "the simulation says X" means

The simulation predicts X given the geometry, material properties, and boundary conditions that were entered. It does not independently verify that those inputs are correct. The burden of verifying inputs is on the analyst. A result produced from incorrect inputs is a precisely computed wrong answer.

Exporting results

  • Images: use the ANSYS result plots directly. Label each with result type, units, and scale range. Set the scale range explicitly — the auto-scale compresses to the data range and may hide gradients that are important at the design limit.
  • Reports: Mechanical → Solution → Report Preview generates an HTML report with all active results. Use this for formal documentation.
  • Tabular data: Solution → Export exports nodal or element data as CSV for post-processing or direct comparison with measurements.