Nonlinear Static Stress

Overview#

Linear static stress breaks down when the physical response is not proportional to load. Autodesk says a Nonlinear Static Stress study should be used whenever a source of nonlinearity is introduced. It names four common forms and states which Fusion supports:

• Material nonlinearity: plasticity, hyperelastic materials such as rubber, and other nonlinear stress-strain behavior. Supported.
• Geometric nonlinearity: large displacements or rotations (a fishing pole bending). Supported.
• Load nonlinearity (follower forces, where load area or orientation changes with deformation): Autodesk says Fusion does not currently support it.
• Boundary condition nonlinearity: Autodesk lists contact that changes during the simulation as an example, but its Nonlinear Static Stress topic says Fusion does not currently support boundary condition nonlinearity, while its study-types topic lists changing contact as something this study simulates. Check the contact types offered in your study.

The load is applied gradually over multiple increments (ramping), which lets the solver account for changing material stiffness and geometry. Autodesk warns that too few increments can cause convergence problems, and too many increase solution time and output size. It is the right choice when you need to know whether a part permanently deforms or how it behaves beyond yield.

Licensing: Nonlinear Static Stress is an advanced study that costs 6 tokens per solve, or is 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 select Nonlinear Static Stress.
• Number of Steps: right-click the study in the browser > Settings (or Manage > Settings). The default is 10 steps.
• Plastic and other nonlinear materials: Setup tab > Materials panel > Manage Physical Materials opens the Material Browser. Choose a material from the Fusion Nonlinear Material Library, or Copy to Favorites and Edit, enable Advanced Properties, and choose Type Plastic (or elastic nonlinear / hyperelastic types).

Step by step#

1. Create a Nonlinear Static Stress study.
2. Assign a nonlinear material. For Plastic, enter stress-strain points above the initial yield (the first two points are generated from the no-stress and Initial Yield Stress points), keep data in ascending order, avoid negative slopes (they can prevent convergence), and choose a Hardening Rule and a Yield Criterion. A material without plastic data stays elastic.
3. Define constraints and loads as for static stress; the load is ramped over the number of steps.
4. Set contacts. Contact types available are Bonded, Offset Bonded, Separation, Sliding, Rough and No Contact (Free). A Coefficient of Static Friction can be added to Separation contact; add it only if it matters, as general experience is that friction slows convergence.
5. In study settings, set the Number of Steps (default 10; the Settings dialog also has Number of Result Intervals options for event studies only).
6. Mesh carefully. Plastic zones need fine elements; use local refinement at expected yielding.
7. Run Pre-check, then solve. Solves run in the cloud; keep the model small to limit time and the risk of hitting Autodesk's model-size and timeout limits.
8. Monitor Job Status. A failed job is refunded; open Details to see the error.
9. In Results (standard viewer), check Safety Factor, Stress, Displacement, Reactions, Strain, Contact pressure and Contact force; use the Step slider and the Transient Results Plot for the evolution over steps.
10. To estimate permanent set, general practice is to include an unloading step; check whether your study offers one, as Autodesk's setup topic does not describe it.

Options reference#

Tips and pitfalls#

Tip: First solve the linear version. If it already looks wrong, the nonlinear one will not fix it. Use the linear result to estimate where the peak load will be and set steps accordingly.

Warning: Autodesk notes too few increments can cause convergence issues, especially when stiffness, geometry or contact change dramatically. General practice: increase the Number of Steps, check for rigid-body motion before contact closes, and check element quality.

Tip: In the plastic range stress rises only slowly with strain, so look at Strain as well as Stress to see how much permanent deformation occurred, and compare it with the elongation of your material from its datasheet.

Warning: Nonlinear results do not superpose. Doubling the load does not double the response. Each load case must be solved separately.

Tip: Keep the model small: symmetry, local sub-models and simplified bolts pay off greatly in nonlinear runs.

Warning: Nonlinear static stress costs 6 tokens per solve, twice a basic study. Failed jobs are refunded (Autodesk FAQ), but a cancelled job is refunded only if no results are available yet. Test with a coarse mesh first.

Practice exercise#

Model a 5 mm thick steel strip with a 10 mm hole, 100 mm long, fixed at one end and pulled at the other. Solve linear static stress at a load producing nominal stress near yield. Then solve the same in Nonlinear Static Stress at twice that load. Expected result (general behavior): the linear model shows stress exceeding yield at the hole; the nonlinear model shows stress limited near yield with a region of permanent strain, and displacement larger than the linear model predicts.

Worked example: a bent clip that yields#

All values here are illustrative assumptions, not Autodesk data. A spring-steel-like clip is a 1 mm thick, 10 mm wide strip, 40 mm long cantilever, deflected 6 mm at the tip. Material: E = 200 GPa, yield 350 MPa, tangent modulus 2 GPa (bilinear hardening).

1. Linear estimate: for a tip displacement delta, F = 3 E I delta / L^3 with I = 10 x 1 / 12 = 0.833 mm^4: F = 3 x 200000 x 0.833 x 6 / 64000 = 46.9 N. Root stress = 6 F L / (b t^2) = 6 x 46.9 x 40 / (10 x 1) = 1125 MPa. That is more than three times yield, so a linear study would report a stress that cannot occur.
2. Nonlinear study: prescribe a 6 mm displacement at the tip (displacement control is more stable than force control for this problem), with 20 load steps (Number of Steps). Expect root stress to plateau close to 350 MPa plus a small hardening contribution and a plastic zone that grows from the root outwards along about a third of the length.
3. Unload (if your study setup allows an unloading step): the tip would stay displaced by a permanent set; the rebound is the elastic recovery. The exact amount depends on the material model and is not given here.
4. Interpretation: yield strain = 350 / 200000 = 0.00175; the elastic root strain at 6 mm deflection would be 1125 / 200000 = 0.0056, about 3.2 times the yield strain, so the plastic zone is substantial. Check that equivalent plastic strain is far below the elongation at break (for spring steel, a few percent) but flag low-cycle fatigue if the clip will be flexed repeatedly.

Design remedies: a longer or thinner clip lowers strain; at 1 mm thickness the maximum elastic deflection is delta_max = sigma_y L^2 / (3 E t / 2) = 350 x 1600 / (3 x 200000 x 0.5) = 1.87 mm. Doubling the length quadruples that to 7.5 mm.

Choosing load steps#

Autodesk's guidance is qualitative: the default is 10 steps; too few causes convergence problems when material stiffness, geometry or contact change dramatically, and too many lengthen the solve and enlarge the output. General practice (not Autodesk data) is to raise the step count for contact-heavy or large-rotation problems and to use prescribed displacement rather than force near a peak load. A model that converges with more steps but not with fewer is telling you the increments were too coarse, not that the physics is wrong.

Material data for plasticity#

Take yield, ultimate strength, hardening and elongation from your material datasheet or tests, or from the Fusion Nonlinear Material Library. As an illustration of estimating a bilinear tangent modulus (general method): (ultimate - yield) divided by the plastic strain at ultimate; for 6061-T6 with typical handbook values of 276 and 310 MPa and an assumed plastic strain of about 0.08 this gives about 425 MPa. For printed polymers the stress-strain curve is far from bilinear; use measured data where the result matters.

Interpreting results by step#

Scrub the Step slider and note the step at which first yield appears and the load fraction at which the plastic zone spans the section. General beam theory (not Autodesk data): full plastic collapse of a bending beam occurs at about 1.5 times the first-yield load for a rectangular section (shape factor 1.5) and 1.7 for a round bar, which is a quick sanity check.

Plastic strain limits#

Autodesk does not give plastic strain limits. Use your material elongation data and design standards, and avoid significant plasticity per cycle in cyclic loading because of low-cycle fatigue (general engineering knowledge).

Failure modes and fixes#

Practice exercise#

Reproduce the clip.

1. Model a 40 x 10 x 1 mm strip, fixed at one end; define a custom steel with assumed E 200 GPa, yield 350 MPa and a plastic stress-strain table consistent with a tangent modulus near 2 GPa.
2. Predict first-yield deflection: 1.87 mm, and the elastic force at 6 mm (46.9 N, not reached because of yielding).
3. Run a linear static study with a 6 mm prescribed displacement and note the root stress (about 1100 MPa).
4. Run the nonlinear study with 20 steps and the same displacement; record root stress, plastic strain and reaction force at the end.
5. If your setup allows an unloading step, record the permanent set. State whether the clip would still clip, and whether repeated use is safe.

Related#

• Static Stress Study
• Contacts
• Event Simulation
• Cloud Solve and Credits