For general information, see Establish Analysis Settings in the Mechanical User's Guide.
The basic analysis settings for Explicit Dynamics analyses are:
Step Controls - The required input for step control is the termination time for the analysis. This should be set to your best estimate of the solution time required to simulate the event being modeled. You should normally allow the solver to determine its own time step size based on the smallest CFL condition in the model. The efficiency of the solution can be increased with the help of mass scaling options. Use this feature with caution; too much mass scaling can give rise to non-physical results.
An Explicit Dynamics solution may be started, interrupted and resumed at any point in time. For example, an existing solution that has reached its End Time may be extended to continue to review the progression of the mechanical phenomena simulated. The Resume From Cycle option enables you to select which Restart file you would like to use to resume the analysis. See Resume Capability for Explicit Dynamics Analyses for more information.
Step Control options:
Number of Steps (option not available in LS-DYNA)
Current Step Number (option not available in LS-DYNA)
Load Step Type (option not available in LS-DYNA)
Resume from cycle (option not available in LS-DYNA)
Maximum Number of Cycles
Reference energy cycle (option not available in LS-DYNA)
The Maximum Element Scaling and Update frequency (options not available in LS-DYNA)
Solver Controls – These advanced controls allow you to control a range of solver features including element formulations and solution velocity limits. The defaults are applicable to wide range of applications.
Shell thickness update, shell inertia update, density update, minimum velocity, maximum velocity and radius cutoff options can only be set in the Explicit Dynamics system.
A selectable Unit System is available only in LS-DYNA.
Euler Domain Controls – There are three sets of parameters that are necessary to define the Euler Domain: the size of the whole domain (Domain Size Definition), the number of computational cells in the domain (Domain Resolution Definition), and the type of boundary conditions to be applied to the edges of the domain.
Note: For information on Euler capabilities supported for LS-DYNA systems, see ALE Workflow in the LS-DYNA User's Guide.
The domain size can be defined automatically (Domain Size Definition = ) or manually (Domain Size Definition = ). For both the automatic and manual options, the size is defined from a 3D origin point and the X, Y, and Z dimensions of the domain.
For the automatic option, specify the Scope of the Domain Size Definition so that the origin and X, Y, and Z dimensions are set to create a box large enough to include all bodies in the geometry (Scope = ) or the Eulerian Bodies only (Scope = ). The automatically determined domain size can be controlled with three scaling parameters, one for each direction (X Scale Factor, Y Scale Factor, Z Scale Factor).
The size of the domain is affected by the scale factors according to the following equations:
(4–1)
(4–2)
(4–3)
where
lx, ly, lz are the lengths of the unscaled domain in the x, y, and z directions respectively. These parameters are obtained automatically from the mesh.
l'x, l'y, l'z are the lengths of the scaled domain in the x, y, and z directions respectively.
Fx, Fy, Fz are the scale factors for the x, y, and z directions respectively.
For the Manual option of the Domain Size Definition, specify the origin of the Euler Domain (Minimum X Coordinate, Minimum Y Coordinate, Minimum Z Coordinate) and the dimension in each direction (X Dimension, Y Dimension, Z Dimension).
The domain resolution specifies how many cells should be created in the X, Y, and Z directions of the domain. Use the Domain Resolution Definition field to specify how to determine the resolution: either the cell size (), the number of cells in each of the X, Y, and Z directions (), or the total number of cells to be created ().
For the Cell Size option, specify the size of the cell in the Cell Size parameter. The value specified is the dimension of the cell in each of the X, Y, and Z directions. The units used for the cell size follow the ones specified in the Mechanical application window and are displayed in the text box.
The number of the cells in each direction of the domain are then determined from this cell size and the size of the domain with the following equations:
(4–4)
(4–5)
(4–6)
where
Nx, Ny, Nz are the number of cells in the X, Y, and Z directions respectively.
D is the dimension of the cell in each direction (this is the same in all directions).
For the Cells per Component option, enter the number of cells required in each of the X, Y, and Z directions (Number of Cells in X, Number of Cells in Y, Number of Cells in Z).
For the Total Cells option, specify Total Cells (the default is 250,000). The size of the cells will depend on the size of the Euler Domain.
The size of the cell is calculated from the following equation:
(4–7)
where
Ntot is the total number of cells in the domain.
If any bodies are defined as Eulerian (Virtual), when Analysis Settings is selected in the outline view, the Euler domain bounding box is displayed in the graphics window. The Euler domain resolution is indicated by black node markers along each edge line of the Euler domain. The visibility of this can be controlled by the Display Euler Domain option in the Analysis Settings.
You can set boundary conditions on each of the faces of the Euler Domain. The faces are labeled Lower X Face, Lower Y Face, Lower Z Face (which correspond to the faces with the minimum X, Y, and Z coordinates) and Upper X Face, Upper Y Face, and Upper Z Face (which correspond to the faces with the maximum X, Y, and Z coordinates). The values of the boundary conditions that can be set for each face are:
Use the boundary condition to flow out material through cell faces. The boundary condition makes the material state of the dummy cell outside the Euler domain the same as that of the cell adjacent to the Flow Out boundary, thus setting the gradients of velocity and stress to zero over the boundary. This approach simulates a far field solution at the boundary, but is only exact for outflow velocities higher than the speed of sound and is an approximation for lower velocities. Therefore, the Flow Out boundary condition is approximate in many cases, and should be placed as far as possible from region of interest and best at a location where the gradients are small.
The boundary condition acts exactly the same as the boundary condition and provides the same results.
Use the boundary condition to prevent flow of material through cell faces. The cell faces are closed for material transport and act as rigid non-slip walls. The Rigid boundary condition takes the material state of the dummy cell outside the Euler domain as a mirrored image of the cell adjacent to the Wall boundary, thus setting the normal material velocity at the rigid wall to zero and leaving the tangential velocity unaffected.
Euler Tracking is currently only By Body, which scopes the results to Eulerian bodies in the same manner as Lagrangian bodies.
Damping Controls – Damping is used to control oscillations behind shock waves and reduce hourglass modes in reduced integration elements. These options allow you to adapt the levels of damping, and formulation used for the analysis being conducted. Elastic oscillations in the solution can also be automatically damped to provide a quasi-static solution after a dynamic event.
For Hourglass Damping, only one of either the Viscous Coefficient or Stiffness Coefficient, is used for the Flanagan Belytschko option - when running an Explicit Dynamics analysis using the LS-DYNA solver, LS-DYNA does not allow for two coefficients to be entered in *CONTROL_HOURGLASS. Thus the non-zero coefficient determines the damping format to be either "Flanagan-Belytschko viscous" or "Flanagan-Belytschko stiffness", accordingly. If both are non-zero, the Stiffness Coefficient will be used.
Note: Linear Viscosity in Expansion options are not supported for LS-DYNA.
Hourglass damping in LS-DYNA is standard by default; in the Explicit Dynamics System the same control is Autodyn Standard.
Erosion Controls – Erosion is used to automatically remove highly distorted elements from an analysis and is required for applications such as cutting and impact penetration. In an Explicit Dynamics analysis, erosion is a numerical tool to help maintain large time steps, and thus obtain solutions in appropriate time scales. Several options are available to initiate erosion. The default settings will erode elements which experience geometric strains in excess of 150%. The default value should be increased when modeling hyperelastic materials. Geometric strain limit and material failure criteria are not present in LS-DYNA.
Output Controls – Solution output is provided in several ways:
Results files which are used to provide nodal and element data for contour and probe results such as deformation, velocity, stress and strain. Note that probe results will provide a filtered time history of the result data due to the relatively infrequent saving of results files.
Restart files should be stored less frequently than results files and can be used to resume an analysis.
Tracker data is usually stored much more frequently than results or restart data and thus is used to produce full transient data for specific quantities.
Output controls to save result tracker and solution output are not available for LS-DYNA.
When performing an implicit to explicit analysis, for a nonlinear implicit analysis, the Strain Details view property must be set to Yes because plastic strains are needed for the correct results.
More information is available in the following sections: