2.10.1. Analysis Settings for Explicit Dynamics Analyses

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).

2.10.1.1. Explicit Dynamics Step Controls

FieldOptionsDescription2DRestart
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.
YesYes
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.YesYes
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.YesYes
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 (%).

YesYes
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.

YesYes
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.

YesYes
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.

YesYes
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.YesYes
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.YesYes
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.

YesNo
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.YesYes
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.

YesYes
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.

YesYes
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.

YesYes
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.

YesYes

2.10.1.2. Explicit Dynamics Solver Controls

FieldOptionsDescription2DRestart
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.

YesNo
Beam Solution Type Bending Any line bodies will be represented as beam elements including a full bending moment calculation.NoNo
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.NoNo
Hex Integration Type Exact Provides an accurate calculation of element volume, even for warped elements. NoNo
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.NoNo
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.NoNo
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.NoNo
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.

NoNo
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/AN/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.NoNo
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

NoNo
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.

YesNo
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.

YesYes
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.

YesYes
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.

YesYes
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.

YesYes

2.10.1.3. Explicit Dynamics Euler Domain Controls

FieldOptionsDescription2DRestart
Domain Size Definition Program Controlled Set Domain Size Definition to automatic.NoNo
Manual Set Domain Size Definition to manual.
Display Euler Domain  Toggles visibility of the annotation of the Euler domain in the graphics window.NoNo
Scope All Bodies Euler domain is sized to include all bodies.NoNo
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 .NoNo
Minimum X Coordinate, Minimum Y Coordinate, Minimum Z Coordinate  X, Y, Z coordinates for the Euler domain origin for the Manual option.NoNo
X Dimension, Y Dimension, Z Dimension  Euler domain X, Y, Z dimensions for the Manual option.NoNo
Domain Resolution Definition Total Cells Set Domain Resolution Definition by specifying the total number of cells in the Euler domain.NoNo
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.NoNo
Cell Size  Dimension of the cell in each of the X, Y, and Z directions if Domain Resolution Definition is Cell Size.NoNo
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.NoNo
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.NoNo
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.NoNo

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.

2.10.1.4. Explicit Dynamics Damping Controls

FieldOptionsDescription2DRestart
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.YesYes
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.YesYes
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.

YesYes
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.

NoYes
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.YesYes
Flanagan Belytschko
Stiffness Coefficient  The Stiffness Coefficient for Flanagan Belytschko hourglass damping in solid hexahedral elements.NoYes
Viscous Coefficient  The viscous coefficient for hourglass damping used in hexahedral solid elements and quadrilateral shell elements.YesYes
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.YesYes

2.10.1.5. Explicit Dynamics Erosion Controls

FieldOptionsDescription2DRestart
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.

YesYes
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.

YesYes
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.

YesYes
On Minimum Element Time Step  If set to Yes, elements will automatically erode if their calculated time step falls below the specified value. YesYes
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.

YesYes
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.

YesNo

2.10.1.6. Explicit Dynamics Output Controls

FieldOptionsDescription2DRestart
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.YesYes
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.

YesYes
Time Save results file after a specified increment in time. Exposes a Time field where you enter a time increment.YesYes
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.YesYes
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.YesYes
Cycles Save restart files after a specified increment in the number of cycles. Exposes a Cycles field where you enter the increment in cycles.YesYes
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.

YesYes
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.YesYes
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.

YesYes
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.

  • Time Increment

  • Energy Conservation

  • Momentum Summary

  • Energy Summary

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.

YesYes
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.

  • Time Increment

  • Energy Conservation

  • Momentum Summary

  • Energy Summary

The Solver Output view from the Solution Output drop down will be updated every cycle.

YesYes
Output Contact Forces  

Use this control to define the frequency that contact forces are written out to file.

  • Contact forces information is written to the solution directory into ASCII files named extfcon_*.cfr, where * is the cycle number.

  • Each file contains forces in the global x, y and z directions for nodes on external faces, where the forces are non-zero.

  • Contact forces are not written for Line bodies or Eulerian (Virtual) bodies.

  • Contact forces are only written for 3D analyses.

  • A separate line pair exists for each node in the following format:

    Node number
    Contact Force X  Contact Force Y  Contact Force Z
  • These text files may be used by ACT to visualize the contact pressure between bodies.

NoYes
Off (Default) Disable output of contact forces.NoYes
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.NoYes
Time Write contact forces to a file after a specified increment in time. Exposes a Time field where you enter a time increment.NoYes
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.NoYes

2.10.1.7. Explicit Dynamics Data Management Settings

Note that these settings cannot be changed from the Details panel.

FieldDescription
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.

2.10.1.8. Recommendations for Analysis Settings in Explicit Dynamics

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 ControlledEfficiencyLow VelocityHigh VelocityQuasi-StaticDrop 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 Factor0.910.90.90.90.9If solving in the Euler reference frame the maximum timestep safety factor is 0.66667. This will override any values entered by the user.
Mass ScalingNoYesYesNoYesNoThe user needs to enter a reasonable desired timestep.
Mass Scaling: Minimum CFL timestepOffUser Must DefineUser Must DefineOffUser Must DefineOffThe 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 (%)Off1000100Off1000Off 
Mass Scaling: Maximum Part ScalingOff10005Off1000Off 
Mass Scaling: Update FrequencyOff00Off0OffNote that for low deformation problems, setting an update frequency of approximately 250 may also help maintain a higher timestep
Characteristic DimensionDiagonalsOpposing FacesOpposing FacesDiagonalsOpposing FacesOpposing Faces 
Solver Controls        
Beam Time Step Safety Factor0.510.10.10.10.1Increasing the safety factor can lead to unstable results. Check results carefully.
Hex Integration TypeExact1pt Gauss1pt GaussExact1pt Gauss1pt Gauss 
Shell Sublayers323333 
Shell Inertia UpdateRecomputeRotateRecomputeRecomputeRecomputeRecomputeRotate option is most efficient but can lead to unstable results. Check results carefully.
Tet IntegrationANPSCPNBSANPNBSNBSSCP tet is very efficient but suffers from shear and volume locking. Check results carefully if using this option.
Minimum Strain Rate Cutoff1e-101e-100.01e-100.00.0 
Damping Controls        
Hourglass DampingAUTODYN standardAUTODYN standardFlanagan BelytschkoAUTODYN standardFlanagan BelytschkoFlanagan BelytschkoAutodyn standard is not rigid body rotation invariant. Must use Flanagan Belytschko if large rotations are involved.
Static Damping 0000User Must Define0For 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 LimitYesNoNoYesNoNoIf 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 Limit1.50.75Unchanged1.5UnchangedUnchanged 
Output Controls        
Save Results on: Equally Spaced Points202050501050 
Save Result Tracker Data: Cycles1101011010 
Save Solution Output: Cycles1001000100100100100 
Body Interactions: Details options        
Nodal Shell ThicknessNoNoNoNoNoNo 
Body Self ContactYesNoNoYesNoNo 
Element Self ContactYesNoNoYesNoNo 

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



Release 18.2 - © ANSYS, Inc. All rights reserved.