Imports a mesh or problem from an external format.


acuImport [options]


AcuSolve Preparatory Program


AcuImport is a utility program that translates a problem and/or a mesh from a third party format and writes it on disk in a format suitable for running AcuRun.

In the following, the full name of each option is followed by its abbreviated name and its type. For a general description of option specifications, see Command Line Options and Configuration Files. See below for more individual option details:

help or h (boolean)
If set, the program prints a usage message and exits. The usage message includes all available options, their current values, and the place where each option is set.
problem or pb (string)
The name of the problem is specified via this option. This name is used to generate input file names.
file_format or fmt (enumerated)
Export the mesh in this format:
ASCII text format.
Binary format.
import_from or from (enumerated)
Import from this format:
Import from ANSYS database.
Import from Fluent/UNS .cas file.
Import from I-deas universal file.
Import from StarCD format.
import_file_name or file (string)
The name of the file from which the problem and/or mesh is to be imported.
mesh_directory or mdir (string)
The name of the directory to place the mesh files.
split_as_tets or tet (boolean)
Convert the imported mesh to an all-tetrahedron AcuSolve mesh. Currently supported only with -from fluent.
coordinates_scaling_factor or crdfct (real)
Scale the coordinates by this factor.
line_buff or lbuff (boolean)
Flush standard output after each line of output.
verbose or v (integer)
Set the verbose level for printing information to the screen. Each higher verbose level prints more information. If verbose is set to 0 (or less), only warning and error messages are printed. If verbose is set to 1, basic processing information is printed in addition to warning and error messages. This level is recommended. verbose levels greater than 1 provide information useful only for debugging.


To import the Fluent/UNS .cas file -channel.cas, issue the command:
acuImport -pb channel -from fluent -file channel.cas
Alternatively place the options in the configuration file Acusim.cnf as:
problem = channel
import_from = fluent
import_file_name = channel.cas
and issue the command:

The above extracts the mesh data from the Fluent/UNS file channel.cas, and writes the input file -channel.inp plus a number of supporting geometry and boundary condition files. The input can then be edited to incorporate additional data, and subsequently run by AcuRun.

The imported coordinates may be scaled by the factor given by -coordinates_scaling_factor. For example, if the coordinates in a Fluent mesh are given in inches, but an AcuSolve mesh is needed in meters, the following command will do the conversion:
acuImport -pb channel -from fluent -file channel.cas -crdfct 0.0254

Input files from the following formats are imported by this program: Fluent, I-deas and ANSYS. Details of the first two are given below.

Fluent Format

For Fluent format, AcuImport imports a Fluent/UNS .cas file from Fluent Inc. The UNS data sets 10, 12, 13, 2010, 2012, and 2013 are read in their entirety, data set 39 is read to extract names, and data set 37 is read to extract some global parameters. These data sets are converted to coordinate file problem.crd; connectivity files problem.etag.cnn, where etag is the set identification; surface connectivity files problem.etag.stag.ebc, where stag is the surface set identification; and nodal boundary condition files problem.etag.stag.nbc, which are the nodes of the surface files. It also generates an input file problem.inp, where these files are referenced by their appropriate input commands. This input file must be edited to incorporate the appropriate boundary condition values, material models, and so on.

All Fluent meshes, including mixed element types, may be imported by AcuImport. Optionally, the imported mesh may be converted to an all-tetrahedron mesh by specifying -split_as_tets.

I-deas Format

For I-deas format, AcuImport imports an I-deas Universal file, from Structural Dynamics Research Corporation. The following data set are translated:
  • Dataset 164: Units
  • Dataset 790: Load Sets
  • Dataset 791: Restraint Sets
  • Dataset 2411: Nodes - Double Precision
  • Dataset 2412: Elements
  • Dataset 2420: Coordinate System

Datasets 164 and 2420 provide the coordinate transformation, which is used to transform the nodal coordinates and nodal boundary conditions to the global coordinate system. The coordinate system of dataset 2420 must be a Cartesian system, as specified by a 0 value for Record 3 Field 2 (coordinate system type).

Dataset 2411 provides the nodal coordinates which are transformed to global coordinate system and written to the problem.crd file.

Dataset 2412 provides the elements. The elements are separated into element sets based on element shape and material ID. The elements are transferred to files problem.tag.mid.cnn; where tag is one of the element shapes tet4, wedge6, or hex8, as determine from Record 1 Field 1 (fe descriptor ID). Only values 111, 112, and 115 are allowed. mid is the material ID given on Record 1 Field 4 (material property table number).

Dataset 791 provides the nodal boundary conditions. Record 1 Field 2 (restraint type) must be either 1 (nodal displacement) or 2 (nodal temperature). Type 1 translates into boundary conditions on a vector field, and type 2 translates into a boundary condition on a scalar field. The boundary condition variable is extracted from the first token of Record 2 (restraint set name). The (lower/upper) case of this token is ignored. For example, if Record 2 is "velocity at inflow", a velocity boundary condition is assumed. The entire record is used for the user given name of the NODAL_BOUNDARY_CONDITION command. For a scalar field, the boundary condition value is extracted from Record 4 Field 1 (temperature value). For a vector field, Fields 3, 4, and 5 of Record 3 (switches for physical dofs) specify whether or not a vector component (in the coordinate system given by dataset 2420) is specified or not. The boundary condition values are extracted from Record 4 Fields 1, 2, and 3 (displacement for dof 1, 2, and 3).

Dataset 790 provides the element boundary conditions, surface outputs, and turbulence wall surfaces. Record 1 Field 2 (load type) must be 2 (finite element face pressure). The boundary condition variable is extracted from the first token of Record 2 (load set name). The (upper/lower) case of this token is ignored. If this token is surface_output, then the set is translated to a SURFACE_OUTPUT command. If this token is turbulence_wall, the set is translated to a TURBULENCE_WALL command. Otherwise the set is translated to an ELEMENT_BOUNDARY_CONDITION command. In any of these cases, the user given name of the set is the entire string of Record 2. For example, if Record 2 is "pressure on the outflow", a pressure boundary condition is assumed. In all cases, surface files problem.tag.ebc.set.ebc are generated; where tag is either tri3 or quad4; ebc is a sequential count of sets; and set is extracted from Record 1 Field 1 (load set number). The boundary condition value is extracted from Record 4 Field 1 (pressure value on face). If Record 3 Field 1 (face pressure load label) is negative, and the set is translated to an element boundary condition, then the boundary condition of type free is assumed.

The directory where the resulting AcuSolve mesh files are placed can be changed. For example, to place these files in the directory mesh.out use the command:
acuImport -mdir mesh.out