The following sections describe the available properties for the Analysis Settings folder in an Explicit Dynamics analysis. In addition to describing each setting, it is noted whether the setting is available for 2D analyses, and whether it is available on restart (applies to 2D and 3D analyses).
| Field | Options | Description | 2D | Restart |
|---|---|---|---|---|
| Resume From Cycle |
Allows you to select the integration cycle from which to start the solution upon selecting Solve. A cycle of zero (default setting) indicates the solution will clear any previous progress and start from time zero. A non-zero cycle, on the other hand, allows you to revisit a previous solution and extend it further in time. A solution obtained from a non-zero cycle is considered to have been "resumed" or "restarted". Note that the list will only contain non-zero selections if a solve was previously executed and restart files have been generated. When resuming an analysis, changes to analysis settings will be respected where possible. For example, you may wish to resume an analysis with an extended termination time. Changes to any other features in the model (geometry suppression, connections, loads, and so on) will prevent restarts from taking place. See Resume Capability for Explicit Dynamics Analyses for more information. This field is not available for Workbench LS-DYNA. | Yes | Yes | |
| Maximum Number of Cycles | The maximum number of cycles allowed during the analysis. The analysis will stop once the specified value is reached. Enter a large number to have the analysis run to the defined End Time. | Yes | Yes | |
| End Time | (Required input) The maximum length of time (starting from time zero) to be simulated by the explicit analysis. You should enter a reasonable estimate to cover the phenomena of interest. | Yes | Yes | |
| Maximum Energy Error | Energy conservation is a measure of the quality of an Explicit Dynamics analysis.
Large deviations from energy conservation usually imply a less
than optimal model definition. This parameter allows you to
automatically stop the solution if the deviation from energy
conservation becomes unacceptable. Enter a fraction of the total
system energy (measured at the Reference Energy
Cycle) for which you want the analysis to stop.
For example, the default value of 0.1 will cause the analysis to
stop if the energy error exceeds 10% of the energy at the
reference cycle. For Workbench LS-DYNA this field requires a percentage to be entered. Thus the field name changes to Maximum Energy Error (%). | Yes | Yes | |
| Reference Energy Cycle | The cycle at which you want the solver to calculate the reference energy, against
which it will calculate the energy error. Usually this will be
the start cycle (cycle = 0). You may need to increase this value
if the model has zero energy at cycle = 0 (for example if you
have no initial velocity defined). This field is not available for Workbench LS-DYNA. | Yes | Yes | |
| Initial Time Step | Enter an initial time step you want to use, or use the Program
Controlled default. If left on Program
Controlled, the time step will be automatically
set to ½ the computed element stability time step. The
Program Controlled setting is
recommended. For Workbench LS-DYNA if this field is left on Program Controlled, the initial time step will be determined by the solver. | Yes | Yes | |
| Minimum Time Step | Enter the minimum time step allowed in the analysis, or use the Program
Controlled default. If the time step drops below
this value the analysis will stop. If set to Program
Controlled, the value will be chosen as 1/10th
the initial time step. This field is not available for Workbench LS-DYNA. | Yes | Yes | |
| Maximum Time Step | Enter the maximum time step allowed in the analysis, or use the Program Controlled default. The solver will use the minimum of this value or the computed stability time step during the solve. The Program Controlled setting is recommended. | Yes | Yes | |
| Time Step Safety Factor | A safety factor limit is applied to the computed stability time step to help keep the solution stable. The default value of 0.9 should work for most analyses. | Yes | Yes | |
| Characteristic Dimension | Diagonals (default setting) |
The characteristic dimension used to determine the time-step for hex elements will be calculated as the volume of the element divided by the square of the longest element diagonal and then scaled by sqrt(2/3). This field is not available for Workbench LS-DYNA. | Yes | No |
| Opposing Face |
The characteristic dimension used to determine the time-step for hex elements will be based on the minimum distance between opposing faces. Select this option to obtain the optimal time step for hex solid elements. Experience to date has shown that this option can significantly improve the efficiency of 3D Lagrange simulations. However, in certain circumstances when cells become highly distorted, instabilities have been observed causing the calculation to terminate with high energy errors. The correct choice of erosion strain can reduce these problems. It is therefore recommended that users only utilize this option if efficiency is critical. This field is not available for Workbench LS-DYNA. | |||
| Nearest Face |
The characteristic dimension used to determine the time-step for hex elements will be based on the minimum distance between neighboring faces. Experience to date has shown that this option can significantly improve the efficiency of 3D Lagrange simulations. However, in certain circumstances when cells become highly distorted, instabilities have been observed causing the calculation to terminate with high energy errors. The correct choice of erosion strain can reduce these problems. It is therefore recommended that users only utilize this option if efficiency is critical. This field is not available for Workbench LS-DYNA. | |||
| Automatic Mass Scaling | If set to Yes, activates automatic mass scaling and exposes the following options. | Yes | Yes | |
| Minimum CFL Time Step |
The time step that you want to achieve in the analysis. Caution: Mass scaling introduces additional mass into the system to increase the computed CFL time step. Introducing too much mass can lead to non-physical results. Note: Employ User Defined Results MASS_SCALE (ratio of scaled mass/physical mass) and TIMESTEP to review the effects of automatic mass scaling on the model. | Yes | Yes | |
| Maximum Element Scaling | This value limits the ratio of scaled mass/physical mass that can be applied to each
element in the model. This field is not available for Workbench LS-DYNA. | Yes | Yes | |
| Maximum Part Scaling | This value limits the ratio of scaled mass/physical mass that can be applied to an
individual body. If this value is exceeded, the analysis will
stop and an error message is displayed. This field is not available for Workbench LS-DYNA. | Yes | Yes | |
| Maximum Mass Scaling (%) | This value limits the ratio of scaled mass/physical mass that is applied to the whole
model. The ratio is expressed as a percentage. This field is only available for Workbench LS-DYNA. | |||
| Update Frequency | Allows you to control the frequency at which the mass scaling will be calculated
during the solve. The frequency equates to the increment in
cycles at which the mass scale factor will be recomputed, based
on the current shape of the elements. The default of 0 is
recommended and means that the mass scale factor is only
calculated once, at the start of the solve. In parallel solutions the update frequency is always set to 0. This field is not available for Workbench LS-DYNA. | Yes | Yes |
| Field | Options | Description | 2D | Restart |
|---|---|---|---|---|
| Solve Units |
All model inputs will be converted to this set of units during the solve. Results from the analysis will be converted back to the user units system in the GUI. For Explicit Dynamics systems, this setting is always mm, mg, ms.For Workbench LS-DYNA this field is termed Unit System and four systems are available for selection: m, kg, s; mm, ton, s; mm, mg, ms; in, lbf, s. | Yes | No | |
| Beam Solution Type | Bending | Any line bodies will be represented as beam elements including a full bending moment calculation. | No | No |
| Truss | Any line bodies will be represented as truss elements. No bending moments are calculated. | |||
| Beam Time Step Safety Factor | An additional safety factor you may apply to the stability time step calculated for beam elements. The default value ensures stability for most cases. | No | No | |
| Hex Integration Type | Exact | Provides an accurate calculation of element volume, even for warped elements. | No | No |
| 1pt Gauss | Approximates the volume calculation and is less accurate for elements featuring warped faces. This option is more efficient. | |||
| Shell Sublayers | The number of integration points through the thickness of an isotropic shell. The default of 3 is suitable for many applications; however, this number can be increased to achieve better resolution of through thickness plastic deformation and/or flow. | No | No | |
| Shell Shear Correction Factor | The transverse shear in the element formulation is assumed constant over the thickness. This correction factor accounts for the replacement of the true parabolic variation through the thickness in response to a uniform transverse shear stress. Using a value other than the default is not recommended. | No | No | |
| Shell BWC Warp Correction | The Belytschko-Lin-Tsay element formulation becomes inaccurate if the elements are warped. To overcome this, the element formulation has an optional correction to include warping. Setting this correction to Yes is recommended. | No | No | |
| Shell Thickness Update | Nodal | Changes in shell thickness are calculated at the nodes of shell elements. This field is not available for Workbench LS-DYNA. | No | No |
| Elemental | Changes in shell thickness are calculated at the element integration
points. This field is not available for Workbench LS-DYNA. | |||
| Full Shell Integration | Available only for Workbench LS-DYNA. Provides a very fast and accurate shell element formulation. | N/A | N/A | |
| Tet Integration | Average Nodal Pressure | The tetrahedral element formulation includes an average nodal pressure integration. This formulation does not exhibit volumetric locking, and can be used for large deformation, and nearly incompressible behavior such as plastic flow or hyperelasticity. This formulation is recommended for the majority of tetrahedral meshes. | No | No |
| Constant Pressure | Uses the constant pressure integrated tetrahedral formulation. This formulation is more efficient than Average Nodal, however it suffers from volumetric locking under constant bulk deformation. | |||
| Nodal Strain |
When Tet Integration is set to Nodal Strain the Puso Stability Coefficient, field is shown. For NBS models exhibiting zero energy modes, the Puso coefficient can be set to a non-zero value. A value of 0.1 is recommended. See Solver Controls for more information. | |||
| Shell Inertia Update | Recompute | The principal axes of rotary inertia are by default recalculated each
cycle. This field is not available for Workbench LS-DYNA | No | No |
| Rotate | Rotates the axes, rather than recomputing each cycle. This option is more efficient;
however, it can lead to numerical instabilities due to floating
point round-off for long running simulations. This field is not available for Workbench LS-DYNA. | |||
| Density Update | Program Controlled | The solver decides whether an incremental update is necessary based on the rate and
extent of element deformation. This field is not available for Workbench LS-DYNA. | Yes | No |
| Incremental | Forces the solver to always use the incremental update. This field is not available for Workbench LS-DYNA. | |||
| Total | Forces the solver to always recalculate the density from element-volume and
mass. This field is not available for Workbench LS-DYNA. | |||
| Minimum Velocity | The minimum velocity you want to allow in the analysis. If any model velocity drops
below this Minimum Velocity, it will be set
to zero. The default is recommended for most analyses. This field is not available for Workbench LS-DYNA. | Yes | Yes | |
| Maximum Velocity | The maximum velocity you want to allow in the analysis. If any model velocity rises
above the Maximum Velocity, it will be
capped. This can improve the stability/robustness of the
analysis in some instances. The default is recommended for most
analyses. This field is not available for Workbench LS-DYNA. | Yes | Yes | |
| Radius Cutoff | At the start of your calculation, if a node is within the specified radius of a
symmetry plane, it will be placed on the symmetry plane. If a
node is outside the specified radius from a symmetry plane at
the start of your calculation, it will not be allowed to come
closer than this radius to the symmetry plane as your
calculation proceeds. This field is not available for Workbench LS-DYNA. | Yes | Yes | |
| Minimum Strain Rate Cutoff | The minimum strain rate you want to allow in the analysis. If any model strain rate
drops below this value, it will be set to zero. The default is
recommended for most analyses. For low speed or quasi-static
analyses, it may be necessary to decrease this value. This field is not available for Workbench LS-DYNA. | Yes | Yes |
| Field | Options | Description | 2D | Restart |
|---|---|---|---|---|
| Domain Size Definition | Program Controlled | Set Domain Size Definition to automatic. | No | No |
| Manual | Set Domain Size Definition to manual. | |||
| Display Euler Domain | Toggles visibility of the annotation of the Euler domain in the graphics window. | No | No | |
| Scope | All Bodies | Euler domain is sized to include all bodies. | No | No |
| Eulerian Bodies Only | Euler domain is sized to include Euler bodies only. | |||
| X Scale factor, Y Scale factor, Z Scale Factor | User defined scaling factors for the automatically determined X, Y, and Z sizes . | No | No | |
| Minimum X Coordinate, Minimum Y Coordinate, Minimum Z Coordinate | X, Y, Z coordinates for the Euler domain origin for the Manual option. | No | No | |
| X Dimension, Y Dimension, Z Dimension | Euler domain X, Y, Z dimensions for the Manual option. | No | No | |
| Domain Resolution Definition | Total Cells | Set Domain Resolution Definition by specifying the total number of cells in the Euler domain. | No | No |
| Cell Size | Set Domain Resolution Definition by specifying the size of the cells in the Euler domain. | |||
| Cells per Component | Set Domain Resolution Definition by specifying the number of cells in each dimension in the Euler domain. | |||
| Total Cells | Total number of cells that the Euler domain should contain if Domain Resolution Definition is Total Number of Cells. | No | No | |
| Cell Size | Dimension of the cell in each of the X, Y, and Z directions if Domain Resolution Definition is Cell Size. | No | No | |
| Number of Cells in X, Number of Cells in Y, Number of Cells in Z | Number of cells required in the X, Y, and Z directions if Domain Resolution Definition is Number of Cells by Component. | No | No | |
| Lower X Face, Lower Y Face, Lower Z Face, Upper X Face, Upper Y Face, Upper Z Face | Flow Out (Default setting) | Specify the boundary condition of the selected Euler domain face to be Flow Out. | No | No |
| Impedance | Specify the boundary condition of the selected Euler domain face to be Impedance. | |||
| Rigid | Specify the boundary condition of the selected Euler domain face to be Rigid. | |||
| Euler Tracking | By Body | Results may be scoped to Eulerian bodies in the same way as for Lagrangian bodies. | No | No |
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, as shown below.

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.
| Field | Options | Description | 2D | Restart |
|---|---|---|---|---|
| Linear Artificial Viscosity | A linear coefficient of artificial viscosity. This coefficient smooths out shock discontinuities over the mesh. Using a value other than the default is not recommended. | Yes | Yes | |
| Quadratic Artificial Viscosity | A quadratic coefficient of artificial viscosity. This coefficient damps out post shock discontinuity oscillations. Using a value other than the default is not recommended. | Yes | Yes | |
| Linear Viscosity in Expansion | Artificial viscosity is normally applied to materials in compression only. This
option allows you to apply the viscosity for materials in
compression and expansion. This field is not available for Workbench LS-DYNA. | Yes | Yes | |
| Artificial Viscosity for Shells | Apply artificial viscosity to all shell elements in addition to solid
elements. This field is not available for Workbench LS-DYNA. | No | Yes | |
| Hourglass Damping | AUTODYN Standard | The method of hourglass damping to be used with solid hexahedral elements. The AUTODYN Standard option is available For 2D analyses only. | Yes | Yes |
| Flanagan Belytschko | ||||
| Stiffness Coefficient | The Stiffness Coefficient for Flanagan Belytschko hourglass damping in solid hexahedral elements. | No | Yes | |
| Viscous Coefficient | The viscous coefficient for hourglass damping used in hexahedral solid elements and quadrilateral shell elements. | Yes | Yes | |
| Static Damping | A static damping constant may be specified which changes the solution from a dynamic solution to a relaxation iteration converging to a state of stress equilibrium. For optimal convergence, the value chosen for the damping constant, R, may be defined by: R = 2*timestep/T where timestep is the expected average value of the timestep and T is longest period of vibration for the system being analyzed. | Yes | Yes |
| Field | Options | Description | 2D | Restart |
|---|---|---|---|---|
| On Geometric Strain Limit | If set to Yes, elements will automatically erode if the
geometric strain in the element exceeds the specified
limit. This field is not available for Workbench LS-DYNA. | Yes | Yes | |
| Geometric Strain Limit | The geometric strain limit for erosion. Recommended values are in the range from 0.75
to 3.0. The default value is 1.5. This field is not available for Workbench LS-DYNA. | Yes | Yes | |
| On Material Failure | If set to Yes, elements will automatically erode if a material
failure property is defined in the material used in the
elements, and the failure criteria has been reached. Elements
with materials including a damage model will also erode if
damage reaches a value of 1.0. This field is not available for Workbench LS-DYNA. | Yes | Yes | |
| On Minimum Element Time Step | If set to Yes, elements will automatically erode if their calculated time step falls below the specified value. | Yes | Yes | |
| Minimum Element Time Step |
The minimum controlling time step that an element can have. If the element time step drops below the specified value, the element will be eroded. | Yes | Yes | |
| Retain Inertia of Eroded Material |
If all elements that are connected to a node in the mesh erode, the inertia of the resulting free node can be retained if this option is set to Yes. The mass and momentum of the free node is retained and can be involved in subsequent impact events to transfer momentum in the system. If set to No, all free nodes will be automatically removed from the analysis. | Yes | No |
| Field | Options | Description | 2D | Restart |
|---|---|---|---|---|
| Save Results on | During the solve of an Explicit Dynamics system, results are saved to disk at a frequency defined through this control. The following settings are available. | Yes | Yes | |
| Cycles | Save results files after a specified increment in the number of cycles. Exposes a
Cycles field where you enter the
increment in cycles. This setting is not available for Workbench LS-DYNA. | Yes | Yes | |
| Time | Save results file after a specified increment in time. Exposes a Time field where you enter a time increment. | Yes | Yes | |
| Equally Spaced Points | (Default) Save a specified number of result files during the analysis. The frequency is defined by the termination time / number of points. Exposes a Number of Points field where you enter the number of results files required. | Yes | Yes | |
| Save Restart Files on | During the solve of an Explicit Dynamics system, restart files are saved to disk at a frequency defined through this control. The following settings are available. | Yes | Yes | |
| Cycles | Save restart files after a specified increment in the number of cycles. Exposes a Cycles field where you enter the increment in cycles. | Yes | Yes | |
| Time | Save restart files after a specified increments in time. Exposes a
Time field where you enter a time
increment. This setting is not available for Workbench LS-DYNA. | Yes | Yes | |
| Equally Spaced Points | (Default) Save a specified number of restart files during the analysis. The frequency is defined by the termination time / number of points. Exposes a Number of Points field where you enter the number of restart files required. | Yes | Yes | |
| Save Result Tracker Data on |
Use this control to define the frequency at which result tracker data and solution output is saved to disk. Result tracker data objects are scoped to specific regions in a model. Solution output provides a summary of the state of the solution as the solve proceeds. This is shown when Solution Information is highlighted in the project tree. This setting applies to all the selectable views in the Solution Output drop down list located in the Solution Information Details view. This field is not available for Workbench LS-DYNA. | Yes | Yes | |
| Cycles | (Default) Save results tracker and solution output data after
a specified increment in the number of cycles. Exposes a
Cycles field where you enter the
increment in cycles. The default value is 1. If a number less than or equal to 10 is entered for Cycles, then the following plots available from the Solution Output drop down will be updated every 10 cycles unless overall progress has increased by 5% since the last data point (in which case, the plots will be updated at a frequency as close to the entered cycle increment as possible). Results trackers are excluded from this limitation.
The Solver Output view from the Solution Output drop down will be updated at the entered cycle increment. Cycle zero and the final cycle will always be displayed even if it is not a multiple of the cycles entered. | Yes | Yes | |
| Time | Save result tracker and solution output data after a
specified increment in time. Exposes a Time
field where you enter a time increment. Although time based, the frequency of Solution Output update is limited to no more than every 10 cycles. If a time equating to 10 cycles or less is chosen, then the following plots available from the Solution Output drop down will be updated every 10 cycles, unless overall progress has increased by 5% since the last data point (in which case, the output will be updated at a frequency as close to the entered time increment as possible). Results trackers are excluded from this limitation.
The Solver Output view from the Solution Output drop down will be updated every cycle. | Yes | Yes | |
| Output Contact Forces |
Use this control to define the frequency that contact forces are written out to file.
| No | Yes | |
| Off | (Default) Disable output of contact forces. | No | Yes | |
| Cycles | Write contact forces to a file after a specified increment in the number of cycles. Exposes a Cycles field where you enter the increment in cycles. | No | Yes | |
| Time | Write contact forces to a file after a specified increment in time. Exposes a Time field where you enter a time increment. | No | Yes | |
| Equally Spaced Points | Write a specified number of contact force files during the analysis. The frequency is defined by the termination time/ number of points. Exposes a Number of Points field where you enter the number of contact force files required. | No | Yes |
Note that these settings cannot be changed from the Details panel.
| Field | Description |
|---|---|
| Solver Files Directory | The permanent location for all the files generated during a solve. This is a read-only field provided for information. |
| Scratch Solver Files Directory | A temporary location for all files generated during a solve. These files are then
moved to the Solver Files Directory for
completed solves. This is a read-only field provided for
information. See Analysis Data Management in the ANSYS Mechanical User's Guide for more information. This field is not available for Workbench LS-DYNA. |
Explicit Dynamics may be used for a wide range of applications, and a default set of Analysis Settings designed to provide the most robust solution are not necessarily suited to every application. Therefore, the Type setting allows the selection of particular defaults depending on the requirements of the solution. The following options are available:
Program Controlled – This is the default setting with a priority for a robust solution.
Low Velocity – Recommended for low deformation/velocity (<100m/s) analyses.
High Velocity – Recommended for high deformation/velocity (>100m/s) analyses.
Efficiency – Settings for minimum runtime. In some cases, this may have an impact on robustness and accuracy.
Quasi-static – Recommended for quasi-static analyses.
Drop Test – Recommended for drop test analyses.
The exact Analysis Settings values for each of the Analysis Settings Preference Types are shown in the table below. Switching the Type property will update all of the items displayed in the table as indicated. If any of these settings are subsequently changed, then the Type will be indicated as Custom.
| Program Controlled | Efficiency | Low Velocity | High Velocity | Quasi-Static | Drop Test | ||
|---|---|---|---|---|---|---|---|
| Default (Robustness) | Setting for minimum run time (also minimum robustness and accuracy in some cases) | Recommended setting for low deformation/velocity simulations (<100m/s) | Recommended for high deformation/velocity simulations (>100m/s) | Recommended setting for quasi-static simulations | Recommended setting for drop test analyses | ||
| Analysis Settings | Notes | ||||||
| Step Controls | |||||||
| Timestep Safety Factor | 0.9 | 1 | 0.9 | 0.9 | 0.9 | 0.9 | If solving in the Euler reference frame the maximum timestep safety factor is 0.66667. This will override any values entered by the user. |
| Mass Scaling | No | Yes | Yes | No | Yes | No | The user needs to enter a reasonable desired timestep. |
| Mass Scaling: Minimum CFL timestep | Off | User Must Define | User Must Define | Off | User Must Define | Off | The user needs to enter a sensible desired timestep and ensure the physical response is not significantly altered by the additional mass added. |
| Mass Scaling: Maximum Element Scaling Factor (%) | Off | 1000 | 100 | Off | 1000 | Off | |
| Mass Scaling: Maximum Part Scaling | Off | 1000 | 5 | Off | 1000 | Off | |
| Mass Scaling: Update Frequency | Off | 0 | 0 | Off | 0 | Off | Note that for low deformation problems, setting an update frequency of approximately 250 may also help maintain a higher timestep |
| Characteristic Dimension | Diagonals | Opposing Faces | Opposing Faces | Diagonals | Opposing Faces | Opposing Faces | |
| Solver Controls | |||||||
| Beam Time Step Safety Factor | 0.5 | 1 | 0.1 | 0.1 | 0.1 | 0.1 | Increasing the safety factor can lead to unstable results. Check results carefully. |
| Hex Integration Type | Exact | 1pt Gauss | 1pt Gauss | Exact | 1pt Gauss | 1pt Gauss | |
| Shell Sublayers | 3 | 2 | 3 | 3 | 3 | 3 | |
| Shell Inertia Update | Recompute | Rotate | Recompute | Recompute | Recompute | Recompute | Rotate option is most efficient but can lead to unstable results. Check results carefully. |
| Tet Integration | ANP | SCP | NBS | ANP | NBS | NBS | SCP tet is very efficient but suffers from shear and volume locking. Check results carefully if using this option. |
| Minimum Strain Rate Cutoff | 1e-10 | 1e-10 | 0.0 | 1e-10 | 0.0 | 0.0 | |
| Damping Controls | |||||||
| Hourglass Damping | AUTODYN standard | AUTODYN standard | Flanagan Belytschko | AUTODYN standard | Flanagan Belytschko | Flanagan Belytschko | Autodyn standard is not rigid body rotation invariant. Must use Flanagan Belytschko if large rotations are involved. |
| Static Damping | 0 | 0 | 0 | 0 | User Must Define | 0 | For quasi-static analyses, it is recommended that static damping is used, but the value used depends on the configuration of the model. See Explicit Dynamics Damping Controls for more details on selecting an appropriate value. |
| Erosion Controls | |||||||
| On Geometric Strain Limit | Yes | No | No | Yes | No | No | If you expect large deformations and mesh distortions during the simulation, a geometric strain limit of 1.0 to 1.5 will be required for the minimum run time case. |
| Geometric Strain Limit | 1.5 | 0.75 | Unchanged | 1.5 | Unchanged | Unchanged | |
| Output Controls | |||||||
| Save Results on: Equally Spaced Points | 20 | 20 | 50 | 50 | 10 | 50 | |
| Save Result Tracker Data: Cycles | 1 | 10 | 10 | 1 | 10 | 10 | |
| Save Solution Output: Cycles | 100 | 1000 | 100 | 100 | 100 | 100 | |
| Body Interactions: Details options | |||||||
| Nodal Shell Thickness | No | No | No | No | No | No | |
| Body Self Contact | Yes | No | No | Yes | No | No | |
| Element Self Contact | Yes | No | No | Yes | No | No |
When using the Explicit Dynamics analysis system, the Body Self Contact and Element Self Contact settings in the Body Interactions object Details panel should be set to Program Controlled in order for the Analysis Settings Preference Type to have an effect on the Body Interactions objects. If the Program Controlled setting is used, the values of the Body Interactions settings will be as shown in the table.
Note: Consider the following guidelines for setting up other areas of your analysis:
Material Properties
Use simplest Material definition possible
Use Linear Elastic properties unless you need to model non-linearities
Bonds
Only use breakable bonds if you really need to
Meshing
Mesh quality is a critical aspect for model performance and accuracy:
Use Hex Meshes whenever possible
Use the patch independent tetrahedral mesh method to ensure uniform element size and timestep optimization
Avoid small elements unless you need them