Setting up the Physics
Time-explicit dynamic analysis is supported by specialized physics interfaces with settings and functionality tailored for the explicit solution method:
•
 Solid Mechanics, Explicit Dynamics
•
 Truss, Explicit Dynamics
The main differences from the Solid Mechanics and Truss interfaces are:
•
Provides the explicit solver with estimates of the time step
•
Includes the Artificial Viscosity and Mass Scaling features
•
Only linear shape functions for the displacement field
•
Reduced integration used as default
•
Weak constraints are not available
•
Some physics features are not available
See documentation of the
•
The Solid Mechanics, Explicit Dynamics Interface
•
The Truss, Explicit Dynamics Interface
Material Models
The explicit dynamics interfaces only support the isotropic materials models included in Linear Elastic Material and Hyperelastic Material. Most additional material behavior, including nonlinear effects, included by adding subnodes such as Damping, External Strain, External Stress, Plasticity and Damage are available and can be used without restriction.
General recommendations to consider when adding material models:
•
The time step estimate is based only on the elastic material behavior. Be careful when adding subnodes that may cause a stiffening effect.
•
Any source of damping affects the stable time step, see Damping.
•
Do not add complex material behavior to domains where they are of little importance. For example, Plasticity can add a significant cost when solving the model also if there is no plastic deformations since the yield condition still needs to be checked every times step.
Anisotropic behavior can be included by adding one or several Fiber features to the material model.
Loads and Constraints
General recommendations to consider when adding loads and boundary conditions:
•
Point loads and constraints tend to excite hourglass deformations if reduced integration is used. Avoid if possible.
•
Be careful when adding boundary conditions that add stiffness to the model like Spring Foundation. The added stiffness is not accounted for when in the stable time step estimate and can thus cause the solution become unstable.
-
Other boundary conditions that add stiffness include the limited displacement option of Prescribed Displacement and Interior Contact.
-
Pair conditions like Bolt Threaded Contact, Contact and General Contact also add stiffness.
•
Volume forces can be costly to evaluate. For example, Gravity often have negligible effects on short duration events and can often be omitted to reduce the solution time.
•
Apply transient loads smoothly to avoid shocks were not expected.
Constraints added by, for example, Continuity, Prescribed Displacement, Roller, or Symmetry are always implemented as pointwise constraints for explicit dynamics. The constraint handling for explicit solvers in COMSOL Multiphysics has limitations compared to the implicit solver. Most notably, a constraint must not depend on the solution; that is, nonlinear constraints are not supported. A constraint can, however, depend on time. These restrictions are seldom any real limitation for structural mechanics, but two cases that can occur when geometric nonlinearity is enabled are:
•
Identity pairs selected by Continuity must use the material frame for both source and destination
A constraint can be depend on the material coordinates but not the spatial coordinates..
See also Explicit Dynamic Contact Analysis.
Initial Conditions
The time step size restriction of an explicit solver means that it is costly to solve long duration events. If the majority of the event is of little interest it can be excluded from the explicit dynamics simulation by instead starting close the time of interest with initial conditions to account for the preceding time.
A common case where this applies is for a drop test from a specified height under gravity accelerations. Rather than solving for the entire free fall, place the object close to ground and apply an initial velocity corresponding to the free fall. For more complicated cases, it is possible to seamlessly use any solution from another study step as initial conditions to the Explicit Dynamics step.
The Explicit Dynamics interfaces can be used with most standard study steps available in COMSOL Multiphysics. Common study steps to define initial conditions for the explicit dynamics include:
•
The Stationary study step to compute static initial values. For example, initiate contact and friction.
•
The Bolt Pretension study step to initialize bolted connections.
•
The Time Dependent study step to use implicit time-stepping initially.
A Time Dependent study step can also be added after the explicit dynamics step to switch back to implicit time-stepping.
Structural Couplings
The Solid Mechanics, Explicit Dynamics and Truss, Explicit dynamics can be coupled using the Embedded Reinforcement multiphysics coupling.
See Modeling Embedded Structures and Reinforcements for more details.
Multiphysics
The Explicit Dynamics interfaces and study step have limited support for multiphysics simulations. Supported multiphysics i capabilities include
•
The Adiabatic Heating feature to model a local temperature effects caused by dissipation.
•
The Phase-field Damage coupling to model the evolution of damage and cracks. Here the algebraic phase field equations added by the Phase Field in Solids interface are solved implicitly while time-stepping.
•
Values of any dependent variable like temperature not solver for by the explicit dynamics study step can be taken from another solution.
Equation-based modeling
The Explicit Dynamics interfaces support equation-based modeling tools. However, note that no equations or dependent variables added are accounted for in the automatic step size estimate for explicit solvers.