Overview#
A Thermal study calculates the steady-state temperature distribution and resulting heat flow in a design, given thermal loads. A Thermal Stress study combines that temperature field with mechanical loads and constraints to give the stresses caused by nonuniform thermal expansion. Autodesk states that Fusion thermal simulations are steady state: loads and constraints must be independent of time, and the solution is the state after an infinite amount of time. There is no transient (time-dependent) thermal study in the Fusion study list.
Use thermal studies for heat sinks, radiators and electronics (Autodesk's examples). Use thermal stress when a part is constrained while heating, or when temperature gradients or different expansion characteristics produce stress. Autodesk's examples are electronics and automotive parts.
Licensing: Thermal and Thermal Stress are basic studies that cost 3 tokens per solve, or are covered by the Fusion Simulation Extension; only Linear Static Stress cloud solves are covered by the subscription. The Solve dialog shows the live cost. Personal-use availability is not stated in the Simulation help.
Where to find it#
- Simulation workspace > Setup tab > Study panel > New Simulation Study, then Study Type Thermal or Thermal Stress (or the New Study dialog).
- Setup tab > Loads panel > Thermal Loads, then choose the Type: Applied Temperature, Heat Source, Convection, Radiation or Internal Heat. Thermal Stress studies also use Structural Constraints and the structural loads.
- Settings (Setup tab > Manage panel > Settings): Global Initial Temperature (thermal) and Default Stress-free Temperature (thermal stress).
- Results in the browser: Temperature, Heat Flux and Thermal Gradient (plus the structural results in thermal stress).
Step by step#
Thermal study:
- Create a Thermal study.
- Check materials: the material must have thermal conductivity, and a temperature difference must exist for heat transfer to occur.
- Define heat input with Heat Source (a specific power passing through faces, edges or vertices) or Internal Heat (power added to or removed from a body, in W, J/s or Btu/s; optionally per unit volume or as a curve versus temperature).
- Define heat removal and a temperature reference. At least one temperature-based load is required: Applied Temperature, Convection (film coefficient and ambient temperature) or Radiation (emissivity from 0 to 1 and surrounding temperature).
- Review contacts. Thermal studies support only Bonded and Offset Bonded contact. A bonded contact is perfectly conductive unless you enter a Thermal Conductance in W/(m^2 K); blank means infinite conductance.
- Optionally set the Global Initial Temperature. Because the solver is steady state, it only chooses a starting point and does not change the end result; a good guess may improve solve time.
- Generate the mesh if you want to inspect it, run Pre-check, and Solve.
- Review Temperature, Heat Flux and Thermal Gradient.
Thermal stress study:
- Create a Thermal Stress study.
- Apply materials, structural constraints, thermal loads and mechanical loads. All contact types except Free are supported, and Thermal Conductance applies here too.
- Check Default Stress-free Temperature in Settings (default 20 C).
- Solve. Results combine static stress and thermal results: Safety Factor (default), Stress, Displacement, Reactions, Strain, Temperature, Heat Flux, Thermal Gradient, Contact pressure and Contact force.
Options reference#
| Thermal load | Applies to | Notes |
|---|---|---|
| Applied Temperature | Faces, edges, vertices (K, C, F, R) | Locks the entity to a temperature, with unlimited heat generated or removed |
| Heat Source | Faces, edges, vertices (W, Btu/s, J/s) | Specific power passing through the entity; Unit Area option for per-area input |
| Convection | Faces | Film coefficient and ambient fluid temperature; Autodesk quotes 5 to 25 W/m^2 K as a typical natural convection range for air |
| Radiation | Faces | Emissivity/absorptivity 0 to 1 and surroundings temperature; view factor of 1 is assumed and only exchange with the environment is modelled, not surface to surface |
| Internal Heat | Bodies | Constant or temperature-dependent; also available in electronics cooling |
Other settings: Global Initial Temperature (thermal), Default Stress-free Temperature (thermal stress, default 20 C), Thermal Conductance on contacts. Adaptive Mesh Refinement is available for both studies, with Heat Flux or Temperature as baseline results.
Tips and pitfalls#
Warning: A temperature load cannot share an entity with other thermal loads (temperature, convection, radiation, surface heat); the software prevents it. Adjacent faces are allowed, but where they meet the vertex is overconstrained and shows artificially low nearby temperatures. Autodesk suggests a small chamfer or splitting a face to separate the loads.
Warning: A source with no means of removing heat gives an infinite temperature; energy in must equal energy out. A model with no temperature-based load fails to solve and the Solve dialog shows warnings (click Repair).
Tip: Convection coefficient dominates results. Vary it to see sensitivity. Autodesk notes that fans raise h and liquids give higher h than gases.
Warning: Thermal stress with an over-constrained part exaggerates stress compared with a real compliant joint.
Tip: Set the stress-free temperature to the temperature at which the part was assembled or made stress-free; Autodesk notes residual stress may accumulate when operating far below it.
Tip: Radiation can dominate when temperature differences are high or flow is low, because the equation uses temperature to the fourth power.
Warning: Fusion's thermal study has no fluid flow; convection coefficients are inputs. For airflow around electronics, Autodesk offers an Electronics Cooling study (Tech Preview).
Practice exercise#
Model a 60 x 60 x 3 mm aluminium plate (illustrative size) and apply 20 W Heat Source on a 10 x 10 mm patch with Convection on the other faces at an assumed h of 10 W/(m^2 K) and 25 C ambient. Because convection counts as a temperature-based load, no extra Applied Temperature is needed. Compare maximum temperature for a flat plate and a finned version. Expected result: the finned version runs cooler because of the larger convective area. Then create a Thermal Stress study with one edge fixed and observe the distortion.
Worked example: a power transistor on an aluminium plate#
The power, dimensions, h and conductivity below are illustrative assumptions; the formula is standard heat transfer. A regulator dissipates 8 W on a 60 x 60 x 3 mm aluminium plate (k about 167 W/mK) with both faces in still air at 25 C, h = 10 W/m^2K.
- Convective area: two faces of 0.0036 m^2 plus edges of 0.00072 m^2, about 0.0079 m^2.
- Average temperature rise: dT = P / (h A) = 8 / (10 x 0.0079) = 101 K, so about 126 C average.
- Fusion check: 8 W Heat Source on the mounting patch, Convection h = 10 at 25 C on the other faces. The plate should be nearly uniform with a hot spot at the transistor.
- Remedies: h = 50 gives dT = 8 / (50 x 0.0079) = 20 K; ten times the area at the same h gives about 10 K. Re-run to confirm.
Estimating h#
Autodesk gives only the 5 to 25 W/m^2 K natural-convection range for air. For other conditions use a heat transfer reference or measurements; run the study at h, 2h and h/2 and, if the maximum temperature moves a lot, the boundary condition dominates and you should measure.
Thermal stress numbers#
General physics, not Autodesk data: free expansion strain = alpha x dT. Aluminium alpha is about 23e-6 /K; with dT = 100 K, strain = 0.0023 and a 60 mm plate grows about 0.138 mm. If fully constrained, sigma = E x alpha x dT = 68900 x 23e-6 x 100 = 158 MPa (typical E). Differential expansion matters: a steel screw (alpha about 12e-6) in aluminium changes preload by roughly 22 micrometres over a 20 mm clamp length for 100 K.
| Case | Thermal stress behavior |
|---|---|
| Free to expand uniformly | Nearly zero stress, only displacement |
| Constrained at both ends | Compressive stress E alpha dT |
| Uniform temperature but different materials bonded | Stress at the interface |
| Gradient through thickness | Bending distortion and stress |
Heat sources and sinks: practical settings#
- Internal Heat on a body takes total power (W) unless Unit Volume is checked; electronics boards from the Design workspace import THERMALLOSS attributes as Internal Heat loads.
- Applied Temperature idealizes an infinite heat sink; heat flow depends on the mesh near that face.
- Do not apply Applied Temperature and another thermal load to the same face.
- Heat Source can model friction heating, for example on a brake pad face.
Failure modes and fixes#
| Symptom | Cause | Fix |
|---|---|---|
| Solve fails with warnings | No temperature-based load, or only a heat source | Add Applied Temperature, Convection or Radiation; use Repair |
| Temperature is exactly ambient | Zero power or load on a suppressed body | Check the load list |
| Very high peak at the source | Small source area, high power density | Check mesh and source area |
| Thermal stress is huge | Over-constrained or wrong stress-free temperature | Free the part; adjust the stress-free temperature |
| Overcooled node at a face junction | Temperature and convection on adjacent faces share a vertex | Add a chamfer or split a face |
| Heat does not cross a joint | Conductance set too low, or no contact | Check Thermal Conductance and the contact set |
Practice exercise#
- Hand estimate: steady rise of 101 K for h = 10 and 20 K for h = 50 (illustrative values above).
- Model the plate with 8 W Heat Source on a 10 x 10 mm patch and Convection on other faces. Solve for both h values and compare mean and peak temperature.
- Add a Thermal Stress study with one edge fixed and the plate free elsewhere; record displacement and stress.
- Fix the plate on opposite edges and observe the stress rise toward the constrained-expansion estimate of about 158 MPa.
Related#
- Contacts
- Static Stress Study
- Cloud Solve and Credits