Event Simulation

Overview#

Event Simulation solves how a structure responds as loads and motion change over time, including inertia. Use it when the "when" matters: a part dropped onto a floor, a hammer strike, a load that ramps and releases, a moving mechanism pushing on a component, or contact that makes and breaks.

Fusion has two event study types: Dynamic Event Simulation (time-dependent events such as impact, with inertia, where Autodesk says time increments are very small and durations short) and Quasi-static Event Simulation (large motion and contact transitions with loads ramped up gradually, and no inertia). Autodesk describes the dynamic solver as explicit, with time steps commonly on the order of a microsecond or even a nanosecond, so run time is proportional to the number of steps and durations on the order of a second are not tenable.

Licensing: Event Simulation 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 choose Dynamic Event Simulation or Quasi-static Event Simulation.
• In the dynamic study: Rigid Bodies panel > Rigid Body, Materials panel > Study Materials, Constraints panel (Structural Constraint, prescribed displacement or translation/rotation), Loads panel (Transient loads, Initial Linear or Angular Velocity), Contacts panel > Global Contacts and Manage Contacts.
• Settings (Manage > Settings or right-click the study > Settings): General tab (Total Event Duration, Number of Result Intervals), Mesh tab, Damping tab (Rayleigh damping, dynamic only) and Result Output tab, where you choose which result variables are saved before you solve.
• Prescribed motion and transient load magnitudes follow multiplier or magnitude curves whose duration must match the study duration.

Step by step#

1. Create a Dynamic Event Simulation study. Name it with the scenario, for example "Drop onto steel plate".
2. In Settings > General, set Total Event Duration (typically extremely short; the default is 1 millisecond) and Number of Result Intervals (more results mean a larger file). Check the Mesh tab.
3. Specify Rigid Bodies for parts whose strain you do not need. They can translate and rotate (6 degrees of freedom at the centre of gravity) but are not deformed, no stress or strain is calculated for them, they are meshed fully and take part in contact.
4. Assign a nonlinear material from the Fusion Nonlinear Material Library using Study Materials, with density (essential for inertia).
5. Apply structural constraints and, where you know how far a body moves, a prescribed displacement or translation constraint with a multiplier curve. If you know the loads, use a Transient load with Time Dependent (Step Dependent) enabled and a Magnitude Curve.
6. Apply an Initial Linear or Angular Velocity to bodies already in motion in the real scenario (dynamic only). Move impacting bodies close together initially, nearly touching, so the specified duration can be as small as possible; Autodesk says the solver spends as much time on the empty-space steps as on the impact itself.
7. Click Global Contacts to generate contacts (Global Separation Contact is on by default with a Default Friction Coefficient). Disable Allow Self Contact if bodies will not contact themselves, to shorten the solve. Use Manage Contacts to suppress unnecessary pairs.
8. Adjust local mesh settings where appropriate; otherwise the mesh is generated at solve time.
9. Run Pre-check and Solve. Before the analysis, Fusion estimates the run time and warns you if it is too long; Autodesk suggests reducing the duration, simplifying the geometry or coarsening the mesh. Cutting the duration from 1 s to 0.1 s makes the job run about 10 times faster.
10. Review results with the Step slider and animation: Stress (default), Displacement and the other variables you selected in the Result Output tab. Autodesk lists element deletion criteria for event studies if you need failed elements removed.

Options reference#

Tips and pitfalls#

Warning: Results can be very sensitive to contact stiffness and mesh. A peak impact stress is a rough indicator; treat it as order-of-magnitude unless you validate with a test or a drop-test measurement.

Tip: Start with a coarse, short simulation to verify the setup (direction of velocity, contact pairs, gravity sign) before the expensive refined run.

Warning: Do not simulate the full free-fall of a drop. Start a few millimetres above the surface with the impact velocity.

Tip: Use symmetry and trimmed models to reduce cost. Replace components that do not take part in load paths with a Point Mass.

Tip: Check for unrealistic deformation. If elements distort badly, refine the mesh or fix the contact setup.

Warning: Token cost per event solve is fixed at 6 tokens, but run time climbs with duration and mesh size and Autodesk may apply job timeout and model-size limits. A failed job is refunded; a cancelled job is refunded only if no results are available yet.

Practice exercise#

Model a 100 mm x 50 mm x 10 mm aluminium block and a 20 mm thick steel plate below it, with a 1 mm gap (illustrative dimensions). Give the block an initial velocity of 3 m/s toward the plate, use Global Contacts with separation, fix the plate bottom. Run for 2 ms. Expected result: the block compresses against the plate, reaches peak contact force within a fraction of a millisecond to a millisecond, and rebounds. Change the velocity to 6 m/s; for elastic contact the peak force would be expected to rise roughly in proportion to velocity (general mechanics).

Worked example: a drop test on a handheld enclosure#

All values are illustrative assumptions; the energy and wave-speed formulas are standard mechanics, not Autodesk data. A 0.25 kg plastic enclosure (ABS) falls 1.2 m onto concrete, landing on a corner.

1. Impact speed: v = sqrt(2 g h) = sqrt(2 x 9.81 x 1.2) = 4.85 m/s. Kinetic energy = 0.5 x 0.25 x 4.85^2 = 2.94 J, equal to m g h = 0.25 x 9.81 x 1.2.
2. Contact duration: the enclosure deforms about 3 mm on impact; assuming roughly constant deceleration, average stopping force F = E / d = 2.94 / 0.003 = 980 N, and the stopping time is about 2 d / v = 1.2 ms. Peak force is often two or more times the average: 1500 to 2000 N.
3. Model setup: represent the floor as a rigid body or a thick slab with its bottom fixed, set the Initial Linear Velocity to 4.85 m/s toward the corner, and use Global Contacts with a small Default Friction Coefficient. Simulate about 3 ms (a few times the estimated contact time) with a sensible number of Result Intervals.
4. Mass check: the model density times volume should equal 0.25 kg. Add the battery and PCB as Point Masses at their centres, or the impact will be softer than reality. A model that is 50 g light carries 20 percent less energy.
5. Review: plot peak stress against time. In ABS (yield 40 MPa), local yielding at the corner is likely; compare peak strain with the elongation of your material (from its datasheet) and check the stress wave that rings through the part, not just the contact point.

Choosing the time scale and output interval#

Autodesk gives no table of durations; choose the duration to cover just before, during and immediately after the event, and keep the result interval count modest. General guidance (not Autodesk data): a drop impact needs a duration of a few contact times, and a slow quasi-static sequence is better run in a quasi-static study.

The explicit time step is limited by the time a stress wave needs to cross the smallest element: dt = L_min / c, with wave speed c = sqrt(E / rho). For steel, c = sqrt(200e9 / 7850) = 5047 m/s; for 1 mm elements, dt = 0.001 / 5047 = 0.2 microseconds. Simulating 2 ms needs about 10,000 steps. Halving the element size doubles the step count and multiplies the element count by 8, so cost rises roughly 16-fold. For ABS, c = sqrt(2.2e9 / 1050) = 1447 m/s, so steps are 3.5 times longer than steel for the same size.

Material and damping considerations#

Material damping and plasticity dissipate energy; without any dissipation a ball bounces forever. Check the energy balance: kinetic energy lost should appear as strain energy and plastic dissipation.

Contact setup for impacts#

Global Separation Contact lets bodies separate after contact, and the Default Friction Coefficient controls sliding; the friction value is your input from your own data. General guidance: mesh both sides of an interface at similar sizes to limit penetration artifacts, and treat a very stiff target as a Rigid Body, which is cheaper than a deformable mesh.

Quasi-static versus dynamic: which to pick#

Pick Dynamic Event Simulation when inertia matters (impact, drop). Pick Quasi-static Event Simulation for large motion and contact transitions where loads are ramped up gradually and inertia is negligible; initial velocity loads are not available there. A common rule of thumb (general guidance, not Autodesk data) is to treat loading as quasi-static when it is applied much more slowly than the part's longest natural period.

Failure modes and fixes#

Practice exercise#

Run a 1.2 m drop test and check the physics.

1. Create a 100 x 60 x 20 mm block with a density giving 0.25 kg (about 2083 kg/m^3), or use a polymer and add a Point Mass to reach 0.25 kg.
2. Set initial velocity 4.85 m/s toward a rigid floor, tilt the block so a corner leads, and simulate 3 ms with 60 steps.
3. Record peak reaction force, peak von Mises stress and strain (the earlier hand estimate suggests forces of the order of 1000 to 2000 N).
4. Repeat at a 0.6 m drop (3.43 m/s); the energy halves, so deformation and peak force fall by about 30 percent for elastic contact (force scales with velocity).
5. Plot reaction force against time and verify that the area under it (the impulse) equals m (v + v_rebound), the momentum change.

Related#

• Nonlinear Static Stress
• Contacts
• Modal Frequencies
• Cloud Solve and Credits