Static Stress Study

Overview#

Static stress is the workhorse study. It answers: given steady loads that do not change over time, how much does the part deform, how much stress develops, and how far is it from failing? The solver assumes linear behavior, which means:

• Material obeys Hooke's law (stress proportional to strain) and never yields.
• Displacements are small compared to the part size, so the geometry does not change meaningfully as it deforms.
• Loads are applied slowly and held; there is no inertia or vibration.
• Contact between parts is allowed, but Autodesk notes that sliding or separating contact is a nonlinear effect: when you include it in a static stress study the solution becomes iterative. Automatic contacts are Bonded.

When the assumptions hold, static stress is fast, cheap and reliable. When they do not (large deflection, plastic yielding, gaps opening and closing, snap-through), switch to the Nonlinear Static Stress study.

Where to find it#

• Simulation workspace > Setup tab > Study panel > New Study, then choose Static Stress in the New Study dialog (the dialog also opens automatically the first time you enter the workspace).
• The study appears in the browser under a Simulation Model node, with materials, constraints, loads, contacts, mesh and results.
• Static stress is solved in the cloud. Autodesk states your Fusion subscription covers the cost of Linear Static Stress cloud analyses, so no tokens are charged; confirm in the Solve dialog (Settings > Token costs & balances). Personal-use availability is not stated in the Simulation help (see the licensing note on the workspace overview page).

Step by step#

1. Create the study (Static Stress). Optionally click Settings in the New Study dialog (or Setup tab > Manage panel > Settings later) to set the study Name, Remove Rigid Body Modes, Mesh settings and Adaptive Mesh Refinement.
2. Check the model. Optionally use Simplify to remove features, apply symmetry, split faces to confine loads or constraints, or remove bodies you do not need (for example fasteners you will replace with a Bolt Connector). Simplification changes only the simulation model.
3. Assign materials (Materials panel). Simulation materials may differ from the Design workspace materials. Steel, aluminium and plastics have very different Young's modulus and strengths, so check you chose the grade you will actually use. General guidance: 3D-printed parts are usually anisotropic and weaker across layers, so a library entry is only an approximation.
4. Apply constraints. Typically a Fixed constraint on mounting faces. Use Pin (cylindrical faces) or Frictionless where a pin or sliding support better represents reality. Do not over-constrain: a fixed face that in reality is a bolt pattern creates artificial stress concentrations.
5. Apply loads. Use Force (Normal, Angle or Vectors), Pressure for surface loading, Gravity (off by default; enable it from the Loads menu) for weight, Moment for torque, Bearing Load for pin forces. Use a Remote Force to apply a load from a point in space without modelling the lever.
6. Verify contacts if there are multiple bodies. Automatic contacts are Bonded by default (Setup tab > Contacts panel).
7. Generate the mesh (Solve panel > Generate Mesh). Start with the default, then use Local Mesh Control to refine small features. Fusion also meshes automatically when you solve.
8. Run Pre-check and fix issues (optional but recommended).
9. Solve. The study is uploaded, solved on Autodesk's servers and the results are returned; watch Job Status for large models.
10. In Results, the Safety Factor guided result appears first. Also examine displacement (does the shape look right?), reaction force and moment (do they match the applied loads?) and stress. Static stress offers Safety Factor, Stress, Displacement, Reaction Force, Reaction Moment, Strain and Contact Pressure.
11. Run a convergence check: refine the mesh, or use Adaptive Mesh Refinement (Settings > Adaptive Mesh Refinement), and see whether the stress at a consistent location still changes. Autodesk gives 1% or 2% as an example of an insignificant change.

Options reference#

Tips and pitfalls#

Warning: Singularities. A sharp re-entrant corner, a point load or a point constraint yields theoretical infinite stress that grows as you refine the mesh. Do not chase that number. Fillet the corner, spread the load or interpret the stress away from the singular point.

Tip: Compare the sum of reaction forces with the applied load. If they disagree, something is wrong in the setup.

Tip: Use symmetry. If the part and loading are symmetric, model half, split faces if needed and constrain the cut faces against translation normal to the plane (a Frictionless constraint works for planes not aligned with global planes). Autodesk lists symmetry as a way to reduce model size and solution time.

Warning: Safety factor is only meaningful where the material is truly linear. If the stress plot shows values above yield, the true part would deform plastically and the redistribution of stress would change the picture. Use a nonlinear study for such cases.

Tip: Von Mises stress is the metric behind the default Yield Strength safety factor and suits ductile materials such as steel and aluminium. For brittle materials Autodesk points to the Ultimate Tensile Strength criterion, which uses 1st principal stress.

Practice exercise#

Model a 100 mm x 20 mm x 5 mm aluminium cantilever plate. Fix one end, apply 100 N at the free end. Solve. Check the tip deflection against the hand formula delta = F L^3 / (3 E I) with I = b h^3 / 12. Expected result: Fusion should agree closely with the hand formula on a reasonable mesh (the agreement depends on your mesh), and bending stress peaks at the fixed end on the top and bottom faces. Refine the mesh and watch the displacement settle.

Worked example: bracket with numbers#

The dimensions and loads are illustrative assumptions, and the aluminium properties are typical handbook values (use the values in your Fusion material). A shelf bracket from 6061 aluminium (E = 68.9 GPa, yield 276 MPa): a 6 mm thick plate, 40 mm wide, arm 100 mm long, carrying 150 N at 100 mm from the wall, bolted to the wall with two M5 holes.

1. Hand estimate: M = 150 x 100 = 15000 N mm; Z = 40 x 36 / 6 = 240 mm^3; sigma = 62.5 MPa at the root. Safety factor against yield = 276 / 62.5 = 4.4. Tip deflection = F L^3 / (3 E I), with I = 40 x 216 / 12 = 720 mm^4: 150 x 1e6 / (3 x 68900 x 720) = 1.01 mm.
2. In Fusion: fix the two hole cylinders (a Pin constraint with the axial direction free is one alternative to Fixed), apply 150 N on the arm's end face as a force in the -Y direction.
3. Solve on the default mesh. Expect displacement near 1.0 mm and peak stress near the root close to 62.5 MPa plus a local rise at the holes.
4. Check reactions (Reaction Force and Reaction Moment results): the force reaction should total 150 N in +Y and a moment couple through the holes.

If the simulation reports noticeably more deflection than the hand estimate, check whether the holes are modelled as fixed (stiffer, giving less deflection) or pinned (softer), and whether the wall mount compliance matters.

Safety factor settings#

Autodesk defines Safety Factor = Material Strength / Actual Stress, using one of two criteria. Static stress, thermal stress and nonlinear static stress studies produce the Safety Factor result, and it is the default result shown when you first solve.

Interpretation from Autodesk: SF below 1.0 means some failure (permanent deformation or breakage); 1.0 is on the verge of failure; above 1.0 is a margin of safety. Designers frequently strive for a minimum between 1.5 and 6 depending on the application, and Autodesk states it cannot dictate what safety factor you should achieve. Related terms: Design Factor (the minimum your codes require), Safety Factor (the calculated result) and Margin of Safety (SF minus 1). Safety factor visualizations are Traffic Light Plot (default), Below Target and Above Target.

Reduce the strength value in a custom material, or demand a larger design factor, for materials whose real strength is below the datasheet value (for example, 3D-printed parts are often weaker across layers; check your own test data, because Autodesk does not give a percentage).

Symmetry and reduced models#

For a plate symmetric about the XY plane, model half and apply a Frictionless constraint on the cut face (it blocks motion normal to the plane and allows sliding within it). Apply half the load. Check that the half-model reaction forces equal half the full-load reactions. For an axisymmetric part under pure axial load, a quarter model is valid but needs two symmetry planes plus a constraint against axial drift.

Symmetry and reduced models (continued)#

Autodesk describes full symmetry as geometry, constraints and loads all symmetric about one or more planes, constraining translation normal to the symmetry plane on the cut faces. An eighth-symmetry model of a fully symmetric part can be statically stable where the full model is hard to constrain. If the planes do not align with global planes, use a Frictionless constraint. Apply the corresponding fraction of the total load to the reduced model and check the reactions.

Mesh for static stress#

Autodesk's Mesh quality page gives a rule of thumb that parts in bending should have a minimum of four linear elements through the thickness (two parabolic elements give similar results), while parts with mostly membrane stress may need only one. The default Average Element Size is 10 percent of model size and Autodesk's recommended range is 5 to 10 percent. If displacement on a thin part is much smaller than your hand calculation, suspect too few elements through the thickness before suspecting constraints. Use Local Mesh Control to add elements in the bending region (see Mesh Controls).

Reading the three top checks quickly#

These are general practice thresholds chosen for this guide, not Autodesk tolerances.

Multiple load cases#

Static stress and shape optimization studies can hold more than one load case. Right-click the active Study node (or a Load Case node) and choose New Load Case, or Clone Load Case to copy the constraints and loads; activate a case by double-clicking it in the browser. Suppress a load case to exclude it from the solution. Worst-case combinations matter: a bracket that survives 150 N down and 80 N sideways separately may fail under the combination. Add the combination as its own case.

Failure modes and fixes#

Practice exercise#

Reproduce the bracket numbers and then explore sensitivity.

1. Build the 6 mm x 40 mm x 100 mm arm and simulate with 150 N. Record tip deflection (target about 1.0 mm), root stress (62.5 MPa) and safety factor (4.4).
2. Change the constraint at the holes from Fixed to Pin with the axial direction free. Record the change in peak stress at the hole edge.
3. Change the material to a 3D-printed PLA with an assumed reduced strength (use 40 percent of the library value as an arbitrary test case, not an Autodesk figure) and recompute the safety factor.
4. Reduce the thickness to 4 mm and predict the stress (6 x 15000 / (40 x 16) = 140.6 MPa) before solving.
5. Write one paragraph stating which assumption affected the result most.

Related#

• Simulation Workspace Overview
• Loads and Constraints
• Mesh Controls
• Results Interpretation