The“Did You Know?” series aims at helping current and future AcuSolve users to learn more about our CFD solution (which is part of the HyperWorks suite)
“Did You Know?” that the AcuSolve product suite contains a powerful post-processing package known as AcuTrace that can be used to perform particle tracking of massless particles? AcuTrace runs in shared or distributed memory parallel environments and can be applied for steady state and transient datasets to generate streamlines and particle path lines. This product is often used in the chemical mixing industry to visualize mixing patterns, residence times, and concentration levels of various fluids in the manufacturing process.
“Did You Know?
CFD Tetramesh panel and Tetra + BL mesh Read more …
“Did You Know” Before exporting a model from HM in any CFD format it is recommended to organize the elements into meaningful components. For example put the shells defining the inflow boundary in a component called “inflow”.
To generate those CFD relevant components efficiently you can use the following tool, located in BCs -> components -> CFD
”Did You Know”AcuConsole uses a hierarchical data format for it’s database. The specific format that we use is called HDF5. This has a number of implications. Here are some capabilities/characteristics that are associated with this:
1.) When a new database is created, all default parameters associated with the simulation are initialized and saved into it. This is the reason that a newly created database has a non-zero size on disk (even before the user has made any changes to it or loaded any data).
2.) All user actions/changes are saved immediately into the database (i.e. the .acs file). This means that the user should NEVER lose data (in theory, anyhow) if the code crashes, machine crashes, etc. When the save button is clicked, the current database is simply copied to the .acs.bak file. When the user exits, they have the option of not saving the changes to the database. If the user chooses not to save the changes, the .acs.bak file is moved to .acs and the uncommitted changes from the current session are not retained.
3.) Every action that the user performs is saved to the database. When users create multiple meshes in the same session of AcuConsole, this can lead to large database sizes. The disk space associated with the “old” meshes can be released by toggling on the “Compress the database” option when closing a database. It is good practice to use this option. If you would like to compress the database even further, be sure that the following option is turned on: File—>Preferences–>Data Base–>Database compression option=”Gzip=1,shuf”. Note that this will slow down the time it takes to open the database initially, but greatly reduce its size on disk.
“Did You Know” that you can use Boundary Layer Blends flag to improve mesh at sharp corner
s. 
A blunt trailing edge of an airfoil is an excellent example. Attached are two images corresponding to Boundary Layer with blends off and Boundary Layer with blends on with a sweep angle of 15 degrees.
Boundary layer settings are set in Surface Mesh Attributes panel under each of the Surfaces
“Did You Know” that AcuSolve requires a single topology and parent volume for each Simple BC, Element BC, Surface Output, etc. command? This becomes very important when using mixed-element meshes. For example, if you have an inlet surface that has trias and quads, this will get written as two separate Simple BC commands – one for the trias and one for the quads. So if you use a mass_flux, flow_rate, or average_velocity inflow type, you’ll get the defined value for the inlet set of trias and that same value for the inlet set of quads – effectively yielding a higher inflow than desired. You’ll also get a strange inlet profile – the computed profile for the trias and the computed profile for the quads.
There my be other Surfaces where this topological separation creates undesired effects as well.
There are two suggestions to handle this.
1. Split the mesh to all tets – so no more mixed-element boundaries. You can do this in HyperMesh or in AcuConsole (Edit > Mesh 2 Tets.)
2. If you really want to use a mixed-element mesh, then it’s better to use a velocity inflow type and define the constant velocity components, or use User Function to define the desired profile.
Large Meshes
“Did You Know” that the mesh generator in AcuConsole is a stand-alone program and can be run separately if you need to leverage better hardware resources. Say, you are running AcuConsole on your laptop and you need to generate a really large mesh. You can click on Tools->Generate Mesh and turn on ‘Export ams file’ and turn off ‘Launch AcuMeshSim’. This will create a file with .ams as an extension and a folder called CAD.DIR. Then the .ams file and CAD.DIR can be copied to the target machine and acuMeshSim can be executed as follows; Say the file name is pipe.ams, acuMeshSim -pb pipe in the folder containing pipe.ams and CAD.DIR.The resulting mesh, pipe.arm and MESHSIM.DIR, can be copied back to the laptop and imported into AcuConsole.
Meshing
“Did You Know” that if you have clean/closed surfaces that define a closed volume, you can create that volume during the geometry import process of AcuConsole? Simply click ‘On’ to ‘Fill voids in the geometry’ in the Import Geometry panel
(AcuConsole requires a closed volume in order to build a mesh for AcuSolve).
ASCII or Binary file format?
“Did You Know” that AcuConsole allows users to choose between writing their mesh files in ASCII or binary format? By selecting binary format, the file size of MESH.DIR on disk is drastically reduced. Additionally, the time to write the mesh to disk from AcuConsole is greatly reduced and AcuPrep will run faster as less time is spent reading the input.
This feature is very beneficial when working with large models. To choose between ASCII and binary file format, select the appropriate option from File–>Preferences–>Export–>Mesh file type.
Command line arguments
“Did You Know” that AcuConsole supports many command line arguments that you can take advantage of. All AcuSolve tools support similar command line structure. From AcuSolve command window type,
acuConsole -h
acuRun -h
acuSolve -h
etc. to know different command line options.
In AcuConsole, If you want to create a new database and import a parsolid model, pipe.x_t, you can execute,
acuConsole -new pipe.acs -import pipe.x_t
Scripts for automation can also be supplied at command line.
Parametric Databases and Analyses
“Did You Know” that AcuConsole offers a powerful selection of tools for creating parametric databases and analyses? One of the most powerful tools is the ability to define variables and expressions within the “Variable Manager”. The variable manager allows users to create variables and assign values to them. The variables can then be used in expressions for defining boundary conditions, mesh sizes, initial conditions, etc. within the AcuConsole database. This is particularly useful for applications where a value is used more than one time within a database. For example, consider a case where there are multiple walls on which the user wants to generate boundary layer elements. By assigning a variable to the first layer height of the boundary layer (say firstLayerHeight:=1.0e-5), the user can type this variable in the panels entry area for every instance of a wall in the database. Then, whenever the user changes the definition of firstLayerHeight in the variables manager, all settings within the database are updated. The attached images reflect this setup. Note that the variables manager is accessed by clicking on the “x=” icon in the main toolbar of AcuConsole.
Reducing Model Size
“Did You Know” that the model size can be reduced drastically if periodicity of a flow field is leveraged. For example in the turbine section, it is common to only model a sector of the complete device. (view the entire description)
Boundary Conditions
“Did You Know” that AcuSolve contains a set of boundary conditions that automatically sets a boundary layer profile at an inlet boundary? When using the inflow boundary condition types of mass_flux, flow_rate, and average_velocity, AcuSolve computes an appropriate boundary layer profile for the velocity and turbulence fields based on the the distance from no-slip walls, and estimated Reynolds Number. The profile is re-computed at each time step such that deforming meshes are properly accounted for in the calculation. This boundary condition provides a robust method of automatically specifying physically realistic inlet conditions. It is much more realistic than specifying a constant velocity condition for internal flow applications.
Mesh problems
“Did You Know” that if the mesh you got into AcuConsole is neither properly scaled nor properly located, you can use model transformation dialog.
Right click on Model, Select Mesh Op and Transform Coordinates. From this dialog you can Scale, Shift and Rotate the model appropriately.
CAD issues
“Did You Know” that if the CAD model that you are bringing into AcuConsole has been tagged with attributes, you can create the edge, surface and volumes groups using attribute names. Say, In ProE you created an attribute called ALTAIR_TAG on each of the faces and volumes and assign appropriate names, the same names will be extracted and used to group faces and volume regions. Take advantage of different grouping options as this is one of the most time consuming process if the models is too complex with multiple faces and volume regions.
Displaying surfaces
“Did You Know” that AcuConsole provides a mechanism to display surfaces based on Simple Boundary Condition, Solar Radiation Surfaces, Interface Surface, so on. Right click on Model->Surfaces->Show to open up “Display surfaces” dialog. This feature is extremely beneficial to check the model to make sure you have the boundary conditions set correctly, sort out surfaces in the visualization window etc.
Mesh motion
“Did You Know” that AcuSolve supports two different types of mesh motion for deforming mesh simulations? The most general technique is known as Arbitrary Lagrange Eulerian (ALE) mesh motion and requires the solution of a hyperelasticity equation. The second type is known as specified mesh motion. Using this technique, the user is required to specify precisely how each node in the model moves in response to the deforming surface or region. This approach reduces compute time significantly, but is not applicable for all types of simulations.
“Did You Know” that AcuPrep can extract values from environment variables and use them in the input file? This can be very useful for parametric analyses. This functionality can be accessed by using the Env() function.
Env(“VARIABLE_NAME”) causes AcuPrep to read the value defined in $VARIABLE_NAME, then use it wherever it is referenced in the input file.
The following example illustrates this concept.
Consider an input file (pipe.inp) with the following command to set the inlet velocity:
SIMPLE_BOUNDARY_CONDITION(“Inlet”){
…
type = inflow
inflow_type = average_velocity
average_velocity = Env(“AVG_VEL”)
}
To quickly investigate a range of results where the inlet velocity is varied between 1 and 3.5, AcuSolve can be run using the following c-shell script:
#! /usr/bin/env tcsh
set VELOCITIES=( 1.0 1.5 2.0 2.5 3.0 3.5) foreach VAL ( $VELOCITIES)
setenv AVG_VEL $VAL
acuRun -pb pipe -np 4
end
AcuSolve will produce a total of 6 runs for this setup, one for each inlet velocity that is defined. Note that you can use whatever programming/scripting language you prefer to set the environment variables.
