AcuTrace has been enhanced to support tracing of spherical particles having finite mass.  When exercising this option, the particle velocity is no longer governed solely by the local flow velocity.  The motion of the particle is computed by solving a conservation equation that incorporates the mass of the particle, the pressure force, the drag force, the viscous stresses, and the virtual mass force.  The user is given control over which terms in the conservation equation should be included at run time and various drag laws are available to choose from.  Wall/particle interactions are handled with user-specified coefficients of restitution to define the energy loss as a result of the collision.

In addition to supporting finite mass particle tracing, the bi-directional coupling between AcuSolve and AcuTrace also provides support for momentum exchange.  For the case of bi-directionally coupled finite mass particle tracing, the effect of the particle's presence appears in the AcuSolve flow field.  The momentum of each particle is computed, and the corresponding reaction force is added to AcuSolve as a source term in each element that the particle passes through.

Note that particles are limited to idealized, spherical shapes in the current release, and the particles are assumed to constitute a dilute and disperse phase within the fluid.  In addition to this, particle-particle collisions are not yet supported.  As a general guideline for use, it is suggested that the ratio of particle spacing to particle diameter should be on the order of 10 or greater for massless particles and on the order of 100 or greater for finite mass particles.

Common applications for finite mass particle tracing include fluidized bed simulations and other applications involving the transport of small particulates within a flow field.

The 14.0 release contains major improvements to the SST and k-omega turbulence models within AcuSolve.  The new formulation improves the accuracy and robustness of the models by incorporating a change of variables for the omega equation.  Instead of solving for the standard k and omega equations, the new formulation solves for k and .  The change of variables does not alter the results produced by the underlying turbulence model, but does have significant benefits with respect to numerical robustness.  The new formulation has vastly improved near wall behavior; having a much more agreeable wall boundary condition of 0.0 for the omega transport equation, as well as the ability to be managed easier through wall functions.  Internal testing and validation has shown that this change of variables produces far superior behavior of the models in comparison to past releases.

The new models are fully compatible with input files created in older versions of the code.  The nodal initial conditions and boundary condition values are still specified in terms of the eddy_frequency variable.  All conversions to the newly introduced transport quantity ( ) are handled automatically.  The new transport quantity (sqrt_eddy_period) will appear in nodal field outputs along with the kinetic_energy and eddy_frequency variables.  

The revised implementations of SST and k-omega are complete with support for wall functions and wall roughness.  Internal testing has shown that a stretch ratio of 1.3 provides optimal results when using wall functions.

It should be noted that the most efficient solution strategy for these models involves iterating multiple times on the turbulence variables for every iteration of the flow equations.  AcuSolve's AUTO_SOLUTION_STRATEGY command has been updated to reflect this solution strategy.

AcuSolve's Arbitrary Lagrange-Eulerian (ALE) mesh motion technology has historically been based on a hyperelasticity model to control the deformation of the mesh.  Using this approach, the stiffness of a given element is assigned based on the proximity to the motion.  In general, this leads to behavior where the elements closest to the motion exhibit high levels of deformation regardless of their size.  In many cases, this formulation leads to undesirable results.  A new method of computing the motion of the mesh has been introduced in AcuSolve V14.0.  Using the new formulation (i.e. Mesh Quality Metric or MQM), the mesh deforms in such a manner as to maintain the original shape of each element.  Each time the boundaries of the simulation are deformed, the mesh is updated using an algorithm that attempts to optimize the quality of the mesh.  The original shape of the elements is used as the reference for which the mesh was assumed to be of optimal quality.  In practice, this method has a number of benefits over the hyperelastic model.  This technique implicitly retains the shape of elements within the boundary layer, which reduces user burden to constrain near wall nodes to move with deforming surfaces.  Additionally, this method inherently moves large deformations to the larger elements in the domain.  Even with ~5000:1 aspect ratio elements near a deforming wall, the MQM approach retains the structure of the boundary layer elements while absorbing the deformation in the far field elements.  See the images below for an example of the behavior of MQM.  Note that the hyperelastic model required constraints on the boundary layer elements to deform to the level shown, whereas the MQM approach handled the boundary layer elements without additional constraint.

AcuSolve V14.0 now supports the definition of surfaces and volumes using mixed element topology.  In previous releases of the solver, it was necessary to specify all input commands such that only a single parent element set and element type were referenced by each command.  This restriction has been eliminated with the 14.0 release and all solver input commands are functional using the mixed topology input.

Support for the mixed topology input is achieved through the introduction of the SURFACE_SET and VOLUME_SET commands.  With these commands in place, it is now possible to read in the individual surface and volume definitions for later reference in the input file.  Surface sets or volume sets of different topology may then be referenced in a single solver command.

Illustration of mixed topology surface input in AcuSolve.

For example:

# +----------------------------------------------------------------------+

# | Surface sets                                                         |

# +----------------------------------------------------------------------+

SURFACE_SET( "inflow tri3 Fluid wedge6" ) {

   surfaces                            = Read("MESH.DIR/inflow.tri3.ebc.B" )

   shape                               = three_node_triangle

   volume_set                         = "Fluid wedge6"

}

SURFACE_SET( "inflow quad4 Fluid brick8" ) {

   surfaces                            = Read( "MESH.DIR/inflow.quad4.ebc.B" )

   shape                               = four_node_quad

   volume_set                         = "Fluid brick8"

}

# +----------------------------------------------------------------------+

# | Simple Boundary Condition                                            |

# +----------------------------------------------------------------------+

SIMPLE_BOUNDARY_CONDITION( "inflow" ) {

   surface_sets         = {"inflow tri3 Fluid wedge6","inflow quad4 Fluid brick8"}

   type                 = inflow

   inflow_type          = average_velocity

   average_velocity     = 1.0

}

SURFACE_OUTPUT( "inflow" ) {

   surface_sets         = {"inflow tri3 Fluid wedge6","inflow quad4 Fluid brick8"}

   integrated_output_frequency = 1

}

This new capability represents a significant change to the architecture of AcuSolve and is being released in phases.  This first release includes support for all solver commands in the AcuSolve input file, and full post-processing support in AcuTrans, AcuFieldView, AcuProbe, and HyperView.  The new input file format is currently not supported by AcuConsole, HyperMesh, AcuTrace, or AcuFwh.  Support for the new format will be added to the remaining programs in a future release.  Note that AcuSolve continues to support the older, single topology format for all commands as well.  As such, full backward compatibility is retained.

The AcuSolve installation now comes equipped with tutorials that provide detailed instructions for getting started with the code and working with some of the more commonly used features.  The purpose of the document is to provide self contained sets of exercises and instructions for both new and experienced users of the software.  The tutorials provide a brief overview of each simulation that is covered, along with the instructions on how to properly set the model up.  All prerequisite files necessary to perform the simulations are included.  The instructions within each tutorial include details on the meshing, solver settings, as well as post-processing of the model.  

As with other AcuSolve documentation, the tutorials are available from the AcuSolve Help Welcome page.  All files necessary to run the simulations that are described in the document are available in the distribution within the following directory: <installation_directory>/model_files/tutorials/AcuSolve>.  The current version includes 5 tutorials, ranging in complexity from steady, isothermal flow to externally coupled multi-physics applications.  Additional tutorials will be added in future releases of AcuSolve.

A newly developed smoothing algorithm has been added to interpolated mesh motion (MMI).  The impact of smoothing is to improve the behavior of MMI when the background mesh introduces local oscillations in the displacement in the mesh.  This option reduces the likelihood of elements collapsing and also smooths the overall displacements that are enforced by MMI.  It should be noted that this feature does have some additional implications.  Under these conditions, the interpolated mesh motion algorithm is allowed to modify the position of any node that has MMI applied to it.  For degrees of freedom that are not entirely constrained by the MMI, the smoothing algorithm can modify the position.  For example, the behavior of mesh_displacement_type = slip is now different for surfaces that are part of an element set that contains an interpolated mesh motion.  The unconstrained degrees of freedom (in the wall parallel direction) are now controlled by the smoothing algorithm and can have non-zero displacement.

AcuSolve's SIMPLE_BOUNDARY_CONDITION command was developed as a mechanism to automate the application of suitable constraints to represent common types of physics.  Inlets, walls, and outlets are examples of the common physics that are addressed by SIMPLE_BOUNDARY_CONDITION.  As part of this command, the constraints that dictate the mesh motion were also added.  Although this does provide a convenient way of assigning constraints, it can introduce some restrictions in flexibility.  To alleviate this, a new command has been created that separates the mesh motion constraints from the SIMPLE_BOUNDARY_CONDITION command.  The new command, MESH_BOUNDARY_CONDITION, provides a centralized mechanism for assigning mesh motion constraints that were previously associated with the SIMPLE_BOUNDARY_CONDITION, FREE_SURFACE, and EXTERNAL_CODE_SURFACE commands. To accomplish this, AcuPrep internally creates a table of constraints for each element face/node on the boundaries and identifies conflicts within the mesh motion boundary conditions.  These conflicts may arise due to combinations of MESH_BOUNDARY_CONDITION and the legacy commands that provide similar functionality.  In the case of conflicting constraints that have equal precedence values, the MESH_BOUNDARY_CONDITION is given priority.  If the precedence values are not equal, then the higher precedence constraint is enforced.  AcuPrep also checks for compatibility of the mesh motion boundary conditions on each node with the boundary conditions applied for the physics through the SIMPLE_BOUNDARY_CONDITION command.

An example showing how to use the newly introduced command to define a planar_slip mesh motion constraint is as follows:

}

The introduction of the MESH_BOUNDARY_CONDITION command deprecates the FREE_SURFACE and EXTERNAL_CODE_SURFACE commands.  In addition to consolidating commands, the MESH_BOUNDARY_CONDITION implementation contains more complete error checking.  Surfaces that are defined as planar_slip (equivalent to mesh_displacement_type=slip in SIMPLE_BOUNDARY_CONDITION) are now checked to ensure that a consistent normal direction exists for the entire surface set.  Full details of the command, along with all supported options, are included in the AcuSolve Command Reference Manual.

The MESH_BOUNDARY_CONDITION command is currently supported within the solver and post-processing programs.  Full GUI support will be added in a future release.  Note that AcuSolve continues to support the legacy commands that provided control over mesh motion boundary conditions.  As such, full backward compatibility is retained.

AcuSolve now supports running in distributed memory parallel mode across multiple Windows hosts.  In the past, this could only be achieved when running on a Windows HPC Server cluster.  This restriction has been lifted, and it is now possible to run in parallel on multiple Windows hosts using Intel MPI, Platform MPI, MS-MPI, and MPICH2.  It should be noted that some set-up work is required to install services and create shared directories.  Please see the HyperWorks Installation manual for further instructions.

As part of this effort, the process of setting up parallel simulations for single host applications has been simplified as well.  It is no longer necessary to install the SMPD daemon for Intel MPI when running in parallel on a single Windows host.

AcuSolve 14.0 comes equipped with a new version of AcuFieldView that is based on Intelligent Light's most recent release of FieldView.  This release of AcuFieldView provides significant improvements when working with AcuSolve data.  The AcuSolve direct reader has been updated to provide full support for mixed element topology surfaces.  In addition to this enhancement, the performance of the direct reader has been improved dramatically.  The performance improvements have been accomplished through a combination of code changes as well as newly added options that enable the user to skip compute intensive steps that are not necessary for all simulations.  Some of the changes that have been made include an ability to avoid reading of AcuSolve's extended output variables.  Disabling this option alone can improve read times by as much as 2x.  User's have the option to remove duplicate surfaces as well, which brings consistency with AcuTrans.  Please see the AcuFieldView User Guide for full details.

Multiple images displaying custom color maps and a multi-window layout.

AcuSolve 14.0 contains a number of other notable changes that are worthy of mention.  A brief description of each is shown below:

The AUTO_SOLUTION_STRATEGY command now solves the mesh stagger first when performing simulations with mesh motion present.

The following table summarizes the changed or newly introduced AcuSolve input file commands.  Note that a full description of each command is available in the AcuSolve Command Reference Manual.

The following table summarizes the AcuSolve input file commands that are deprecated in this release.  Support will continue for legacy input files, but users should migrate their modeling process to leverage the new commands when possible.

The following table summarizes the changed or newly introduced AcuSolve command line arguments.  Note that a full description of each option is available in the AcuSolve Programs Reference Manual.