Overview#
The Simulation workspace lets you test a digital model before you build it. You apply forces, supports, temperatures and material properties to a design, Fusion divides the geometry into a mesh of small elements, a solver calculates how each element responds, and you read the result as colored contour plots, numbers and animations. The aim is to answer engineering questions early: Will this bracket yield? Will it ring at the motor frequency? Will this heat sink keep the chip under its maximum temperature? Does the buckling load of this strut exceed what I plan to put on it?
Simulation does not replace testing. It produces an estimate whose quality depends on how well your setup represents reality. A beautifully colored plot from a badly constrained model is worse than no plot, because it looks authoritative. This section teaches both the mechanics of each study type and the judgment needed to trust the answer.
Study types listed in Autodesk's "Fusion study types" topic (the topic notes that Electronics Cooling is in Tech Preview):
| Study type | Question it answers | Cloud cost (Autodesk token page) |
|---|---|---|
| Static stress | Stress, displacement, safety factor, reactions under steady loads (linear, small deformation) | Covered by your Fusion subscription |
| Modal frequencies | Natural frequencies, mode shapes and mass participation factors | Basic study: 3 tokens, or Simulation Extension |
| Thermal | Steady-state temperature and heat flow (Fusion thermal studies are steady state only) | Basic study: 3 tokens, or Simulation Extension |
| Thermal stress | Combined structural and temperature-induced stress | Basic study: 3 tokens, or Simulation Extension |
| Shape optimization | Remove material while meeting stress and displacement objectives | Basic study: 3 tokens, or Simulation Extension |
| Structural buckling | Critical buckling multipliers and mode shapes | Advanced study: 6 tokens, or Simulation Extension |
| Nonlinear static stress | Large deformation, changing contact, nonlinear material, permanent deformation | Advanced study: 6 tokens, or Simulation Extension |
| Quasi-static event simulation | Large motion and contact transitions with ramped loads, in single parts or assemblies | Advanced study (Event Simulation): 6 tokens, or Simulation Extension |
| Dynamic event simulation | Time-dependent events such as impact, with load curves and initial velocities | Advanced study (Event Simulation): 6 tokens, or Simulation Extension |
| Plastic injection molding | Fill, visual defects and warpage from process settings | Advanced study: 6 tokens, or Simulation Extension |
| Electronics cooling (Tech Preview) | Component and air temperatures, heat sinks and fans | Advanced study: 6 tokens, or Simulation Extension |
Where to find it#
- Click the workspace menu and select Simulation.
- The first time you bring a design into the workspace, the New Study dialog opens automatically with an icon for each analysis type and a Help Deciding drop-down. Later, use the New Study command in the Study panel of the Setup tab.
- The toolbar has a Setup tab (panels: Study, Simplify, Materials, Constraints, Loads, Contacts, Display, Solve, Manage, Inspect, Select) and, once a study is solved, a Results toolbar (panels include Result Tools, Compare, Deformation and Display). The commands change with the study type.
- The browser shows a Units node, then one or more Simulation Model nodes; each Simulation Model contains Study nodes (default name is a serial number plus the study type), and a Results node indicates whether results are out of date. Use the Activate radio button to change the active model or study.
Step by step#
This is the universal workflow. Later pages show the study-specific details.
- Finish the design. Make a copy of the part or assembly, or use a configuration, so that you can modify it freely for analysis. In the Design workspace, simplified geometry gives better results than detailed geometry.
- Switch to the Simulation workspace and choose New Study. Select the study type. Name it descriptively, such as "Bracket - 500 N downward".
- Review the model. Choose which bodies or components take part, and suppress those that do not matter (screws, cosmetic bodies, cables). A smaller model solves faster and fails less often.
- Assign materials. Each body takes a material from the Fusion library or one you define. Strength, stiffness (Young's modulus), Poisson's ratio, density and, for thermal studies, conductivity and specific heat all matter.
- Add constraints. Remove rigid-body motion by fixing, pinning or otherwise supporting the model. See Loads and Constraints.
- Add loads: forces, pressure, moment, gravity, remote force, bearing load, temperature and so on.
- Check contacts if the model has multiple bodies. Fusion generates automatic contacts, which you should verify.
- Generate the mesh (Solve panel > Generate Mesh) and inspect it. Adjust Mesh Settings or add local mesh controls near stress concentrations. Fusion also meshes automatically when you solve.
- Run Pre-Check (optional but recommended). It checks that the required analysis settings are applied; it only validates that standard inputs are present, so you must still review that the intended simulation is what is being solved.
- Click Solve (Setup tab > Solve panel > Solve), select the studies and, if you have more than one account, the account to charge. Autodesk states that all simulation studies are solved on the cloud; you need a token balance or an active Simulation Extension subscription to solve most studies.
- Review the Results. Switch the result type, adjust the deformation scale, probe values, use the Compare tools, and check mesh convergence.
- Iterate: change the design, the load or the mesh and solve again. Clone or copy the study for variants instead of rebuilding.
Options reference#
Key regions of the workspace:
| Element | What it does | Notes/default |
|---|---|---|
| Study tab | Switches between studies in the same document | Many studies can share one design |
| Browser > Studies | Lists the study tree: model, materials, contacts, constraints, loads, mesh, results | Right-click a node to edit, delete or suppress |
| Simplify (Setup tab > Simplify panel) | Opens the Simplify contextual environment to remove features, use symmetry, split faces and create simulation model variants | Changes stay in the simulation model; the design model is untouched |
| Materials | Assigns physical and structural properties | Simulation materials may differ from the materials defined in the Design workspace |
| Pre-Check | Checks that required settings are applied | Optional, but good practice before a solve; the Solve command shows a status icon (cannot solve, potential issues, no issues) |
| Solve | Cloud solve | Select Token costs & balances in the Solve dialog Settings to see Required, Available and Will Remain |
| Results | Safety factor, stress, displacement, reaction force and moment, strain, contact pressure (static stress) | Available result types vary per study |
| Compare (Results toolbar) | Side-by-side comparison of results with camera, result-type and legend synchronization | Useful for design-iteration work |
| Job Status | Shows running jobs and jobs run in the past 30 days (Simulation and Uploads tabs) | Opens automatically when you launch an analysis; you can close Fusion and results download when you reopen |
Licensing and cost, in summary (from Autodesk's token and extension topics):
- Your Fusion subscription covers the cost of running Linear Static Stress analyses on the cloud. All other studies are solved on a prepaid basis with Flex tokens (3 tokens for basic studies, 6 for advanced studies), or without limits with the Fusion Simulation Extension.
- The features previously offered by the Generative Design Extension are now part of the Simulation Extension.
- Pressing Solve charges tokens; the system consumes them when results become available (for injection molding, when intermediate results become available). Preview functionality currently has no cost.
- Personal-use availability of simulation types, tokens and extensions is not stated in the Simulation or Extensions help.
Note: not confirmed in Autodesk's documentation: which simulation studies or cloud solves a Personal-use licence includes. The help only says that a Personal licence gives Basic Access to hubs other than your own, and that the extension and token availability shown in the Purchase Manager depends on your type of Fusion access. Check the Purchase Manager and Autodesk's current plan comparison.
Tips and pitfalls#
Tip: Make a dedicated analysis copy of your design. Delete holes you do not need, remove cosmetic fillets, and suppress small bolts. Mesh quality improves dramatically.
Tip: Run a rough, low-fidelity solve first. If the high-level result is wrong (the part flies off to infinity, the stress is zero), fix the setup before refining the mesh.
Warning: Simulation assumes the model is linear-elastic unless you use a nonlinear study. Stress above the yield strength is meaningless in linear static stress. The model does not yield; it just reports a number that cannot occur in a real part.
Warning: A solve that converges does not mean the answer is right. Check reaction forces against applied loads and check that the displacement shape looks like what you expect.
Tip: Name loads and constraints. Studies with ten unnamed forces become impossible to debug.
Practice exercise#
Open any simple bracket. Create a Static Stress study. Without applying a load, run Pre-Check and read what Fusion warns about (missing constraint, missing load). Then fix each warning one at a time and run Pre-Check again until it passes. Expected result: you learn what the validator tells you before you ever solve.
Choosing the right study#
| Question | Study | Cheapest check first |
|---|---|---|
| Will it break under a steady load? | Static stress | Hand calculation of beam or axial stress |
| Will a very slender part collapse? | Structural buckling | Euler load |
| Will it ring at the driving frequency? | Modal frequencies | Estimate from a cantilever formula |
| Will it overheat? | Thermal | Power divided by (h x area) for temperature rise |
| Will it distort when hot? | Thermal stress | Free expansion: alpha x L x dT |
| Does it yield, or do parts separate? | Nonlinear static stress | Linear study, then look at stress above yield |
| What happens in a drop or impact? | Event simulation | Impact velocity v = sqrt(2 g h) |
| Can it be lighter? | Shape optimization or generative design | Static stress on the original for a baseline |
A hand estimate takes five minutes and gives you a number to compare with. Example: a steel bar 20 x 5 mm in cross-section, 200 mm long, fixed at one end with 50 N at the tip: M = 50 x 0.2 = 10 N m, section modulus Z = b h^2 / 6 = 20 x 25 / 6 = 83.3 mm^3, stress = 10000 N mm / 83.3 mm^3 = 120 MPa. If the study reports 400 MPa at the root, find the cause before continuing.
The setup-solve-review loop#
General guidance (not Autodesk data): spend most of your effort on geometry preparation, materials, constraints and loads, and only then on mesh tuning. If you find yourself tuning mesh sizes before you have checked reaction forces, step back.
A disciplined sequence:
- Run the coarse, default-mesh version and verify that reactions balance, the deformed shape makes sense and the stress magnitude is in the same range as your hand estimate (a rough rule of thumb, not an Autodesk tolerance).
- Refine only where the result is critical.
- Record the final numbers: load, mesh size, element count, peak stress away from singularities, safety factor.
- Make one change at a time in a cloned study, so differences are attributable.
Units, coordinate systems and results scale#
Fusion simulation uses the unit system of the document, and loads are entered in the units shown in the dialog. A common error is a 100 lbf load entered as 100 N, which is 4.4 times too small. Check the arrow direction in the canvas against the global axes shown in the view cube, since the default Y-up or Z-up orientation of the document may differ from the one in your head. Results display uses a deformation scale (Results toolbar > Deformation panel); always read the displayed scale before judging whether the part "bends a lot".
What the workspace does not do#
- It does not model fatigue life directly; a static safety factor above 1 says nothing about a part under 10 million cycles.
- Structural and thermal studies do not model fluid flow; convection coefficients are inputs. (The Electronics Cooling study, in Tech Preview, does model air flow around electronics.)
- It does not account for manufacturing defects, anisotropy of printed parts or weld heat-affected zones unless you provide those material properties.
- It does not validate itself. Where a result matters for safety, test a physical sample.
Failure modes and fixes#
| Symptom | Cause | Fix |
|---|---|---|
| Pre-Check says model is unconstrained | No constraint, or constraints on suppressed bodies | Add a constraint on an active body |
| Solve fails with a mesh error | Slivers, tiny faces, overlapping bodies | Simplify geometry; remove overlaps; merge close vertices |
| Result is zero everywhere | Load on a suppressed face or zero magnitude | Check the load list and the arrow |
| Result huge and nonsensical | Units mismatch or rigid-body motion | Check units; add the missing constraint |
| Study type missing from New Study | Not available to your type of Fusion access | Check the Purchase Manager and the Simulation Extension status |
| Study works on a copy but not on the original | Original has many tiny features | Simplify the analysis copy |
Practice exercise#
Carry out the full loop on a simple L-bracket.
- Model an L-bracket from 3 mm aluminium sheet, 40 mm per leg, 30 mm wide, with two holes on the base leg. Duplicate the file as
bracket-analysis. - Do a hand estimate (illustrative numbers chosen for this exercise) for 100 N on the vertical leg tip, 40 mm from the bend: M = 4 N m and bending stress at the bend = 6 M / (b t^2) = 6 x 4000 / (30 x 9) = 88.9 MPa.
- Create a Static Stress study, fix the base holes, apply 100 N, solve on the default mesh and compare the peak stress at the bend with 88.9 MPa. Note the difference.
- Add a local mesh refinement at the bend and compare again.
- Clone the study, increase the thickness to 4 mm, and use the Compare tools to quantify the stress drop (from the hand formula, about 44 percent, since bending stress goes with 1/t^2).
Related#
- Static Stress Study
- Loads and Constraints
- Cloud Solve and Credits