Abaqus

This is the documentation for all Abaqus solver wrappers. Abaqus is a structural solver implementing the finite element method. Currently, this wrapper only supports FSI simulations, no other multi-physics problems. Subcycling within the structural solver is possible.

Fluid-structure interaction with Abaqus

Abaqus (Dassault Systèmes) can be used to solve for the structural displacement/deformation in partitioned FSI-simulations. The FSI interface consist of a surfaces in the Abaqus model, where pressure and surface traction loads are applied, and corresponding node sets, where the resulting computed displacements are returned to the solver wrapper. The loads are applied in so-called load points (Gauss points, quadrature points), the displacements are exported in the elements' nodes. The input loads are collected in one or more ModelParts in the input Interface, the output nodes are collected in one or more ModelParts of the output Interface. Each ModelPart on the input Interface has a counterpart on the output Interface. More information about ModelParts and Interface can be found in the data structure documentation.

Terminology

• Main directory: Directory where the analysis is started.
• Working directory: Subdirectory of the main directory in which Abaqus runs.
• Source directory: Directory where the source files of the Abaqus solver wrapper are found: coupling_components/solver_wrappers/abaqus.
• Extra directory: Subdirectory of the source directory with some files to assist with the setup.
• Geometrical nodes: Nodes in Abaqus related to the geometry of the elements. At these nodes the displacement data is exported.
• Load points: Every element has load points. This is where the loads (input to Abaqus) are applied.
• Time step: Time step from the viewpoint of the fluid-structure interaction, usually equal to the time-step of the flow solver and structural solver, although one of the solvers can deviate in the case of subcycling.
• Increment: Time increment in the nomenclature of the Abaqus software. This is usually equal to the time step of the flow solver and overall coupled simulation, but in case of subcycling within the Abaqus solver, a time step can be subdivided in multiple increments.

Environment

• A working directory for Abaqus needs to be created within the main directory. Its relative path to the main directory should be specified in the JSON file. In the CoCoNuT examples this folder is typically called CSM, but any name is allowed.
• The Abaqus software should be available as well as compilers to compile the user-subroutines (FORTRAN) and post-processing code (C++). Some compilers also require a license.
• If the Abaqus license server needs to be specified explicitly, it is advised to do this in the solver modules file.

Parameters

This section describes the parameter settings in the JSON file. A distinction is made between mandatory and optional parameters. It can be useful to have a look at a JSON file of one of the examples in the examples folder.

Mandatory

parameter	type	description
arraysize	int	Size specification for array in FORTRAN part of the code, to reserve sufficient memory. Should be large enough and depends on the number of load points in the structural model.
cores	int	Number of cores to be used by Abaqus.
delta_t	float	Size of the time step in Abaqus. Its value should be synchronized with the flow solver. This parameter is usually specified in a higher Component object in which case it is not mandatory.
dimensions	int	Dimensionality of the problem (2 or 3).
interface_input	list	Should contain a dictionary for each input ModelPart to be created, having a key "model_part" that provides the name of a ModelPart for Abaqus load points as value. The name should correspond to the Surfaces created in Abaqus concatenated with "_load_points". The second key of the dictionary is variables. The list given as value specifies the input variables that should be included, chosen from data_structure/variables.py. Currently only "pressure" and "traction" are allowed. The order of should correspond to the interface_output as well as the other solver wrapper's Interface definitions to which Abaqus is coupled. An example can be found in this part of the input file section.
interface_output	list	Similar to interface_input but contains the output ModelParts for Abaqus geometrical nodes. The name has to correspond to the Node Sets created in Abaqus, concatenated with "_nodes". In this case the "variables" key specifies the output variable, chosen from data_structure/variables.py. Currently only "displacement" is allowed. The order of should correspond to the interface_input as well as the other solver wrapper's Interface definitions to which Abaqus is coupled. An example can be found in this part of the input file section.
input_file	str	Name of the Abaqus input file (.inp) provided by the user. Example: "case.inp"
timestep_start	int	Time step to start from. Data should be available at this time step. For a new simulation this value will typically be 0. This parameter should be synchronized with the flow solver. This parameter is usually specified in a higher Component in which case it is not mandatory to specify.
working_directory	str	Relative path to the directory in which Abaqus will be executed and where all structural information will be stored. Should be created before execution, see the environment section.

timestep_start and delta_t are necessary parameters, but are usually defined in a higher Component. However, they can also be given directly as parameter of the solver wrapper (e.g. for standalone testing). If they are defined both in higher object and in the solver wrapper, then the former value is used and a warning is printed.

Optional

parameter	type	description
debug	bool	Default: false. For every iteration, text files are saved with the input and output data of the solver.
ramp	bool	Default: false. Only used when automatic time incrementation (subcycling) is enabled in Abaqus. false: Load is considered to be constant throughout the time step. true: Load is applied in a ramped fashion throughout the time step.
save_results	int	Default: 1. Determines what output files are kept by Abaqus. Only the .odb files corresponding to (i.e. of which the time step is a multiple of) save_results are kept at the end of a time step.

Overview of operation

The solver wrapper consists of 6 types of files located in the source directory (with X denoting the Abaqus version, e.g. v2022.py):

• abaqus.py: Contains the base class SolverWrapperAbaqus.
• X.py: Defines the SolverWrapperAbaqusXclass, which inherits from the base class. Some version specific parameters might be overwritten in these subclasses.
• abaqus_v6.env: Environment file setting the environment for the Abaqus solver.
• GetOutput.cpp: Extracts the output (from Abaqus .odb files) and writes it to a file for each outputModelPart. Written in C++.
• USR.f: An Abaqus user-subroutine that reads the loads from files (one for each input ModelPart) and applies them on the load points. Written in FORTRAN.
• USRInit.f: An Abaqus user-subroutine that extract the coordinates of the load points and writes them to files (one for each input ModelPart) to initialize each input ModelPart. Written in FORTRAN.

The initialize method

During initialization of the SolverWrapperAbaqusX object, some parameters are substituted in abaqus_v6.env, GetOutput.cpp, USR.f and USRInit.f and these files are copied to the working directory. The C++ files and FORTRAN files are subsequently compiled. USRInit is ran to obtain the coordinates of the load points at the Surfaces defined in Abaqus. These coordinates are stored in ModelParts of which the name corresponds to the entries in interface_input. GetOutput is ran to extract the coordinates of the geometrical nodes. These coordinates are added to ModelParts of which the names corresponds to entries of interface_output. The input ModelParts are added to an Interface object taking care of the inputs (i.e. loads), the output ModelParts to another instance of Interfacetaking care of outputs (i.e. displacements).

Files written in the working directory during initialize

In the file conventions A is the index of the corresponding element in the interface_input or interface_output list.

• The Abaqus input file (input_file in JSON file) is processed into a file CSM_Time0.inp and CSM_Restart.inp, the latter taking care of all simulations (i.e. coupling iterations) but the first.
• Upon running USRInit the load point coordinates of each surface are written to CSM_Time0Cpu0SurfaceAFaces.dat. When these are processed by the solver wrapper, also CSM_Time0SurfaceAElements.dat is created.
• Upon running GetOutput the geometrical nodes are written to CSM_Time0SurfaceANodes.dat.

Note that the CSM_Time0.inp and CSM_Restart.inp are created each initialization (even during restart), however the USRInit and GetOutput are only run when timestep_start equals 0.

The solve_solution_step method

This method of SolverWrapperAbaqusX is called each coupling iteration with an Interface object (input_interface) containing loads, which are written to files that are read by the (compiled) USR.f during the invoked Abaqus simulation. The Abaqus software is started and shut down for each calculation, i.e. each coupling iteration. When the simulation has ran successfully (log-file abaqus.log is checked for errors), the outputs are read from Abaqus by GetOuput and written to a file. The file is read in Python and the output (displacements) are stored in the output Interface object which is returned.

Files written in the working directory during solve_solution_step

In the file conventions A is the index of the corresponding element in the interface_input or interface_output list and B the time step.

• Files written by Abaqus for allowing a restart (required every coupling iteration): CSM_TimeB.odb, CSM_TimeB.res, CSM_TimeB.mdl, CSM_TimeB.prt, CSM_TimeB.stt.
• Output database file written by Abaqus called CSM_TimeB.odb and read by GetOutput (also needed for restart).
• Output text file CSM_TimeBSurfaceAOutput.dat containing displacements written by GetOutput and read by the solver wrapper.
• Input text file CSM_TimeBSurfaceACpu0Input.dat containing the loads written by the solver wrapper and read by the USR.

The parameter save_restart (defined at the level of the coupled_solver) determines at which time steps these files are saved. Additionally, the save_results parameter defines the rate at which the output database files (.odb) are kept.

Setting up a case: Abaqus input file (.inp)

The Abaqus solver wrapper is configured to start from an input file which contains all necessary information for the calculation. This file should be located in the main directory. Its name should be specified in the JSON file via the parameter input_file. For the remainder of this section this file will be referred to as "base-file".

Creation of the base-file is not considered a part of the solver wrapper functionality as it is case-specific. However, in order for the solver wrapper to work, the base-file has to comply with certain general conditions. This section aims at informing the user about the requirements for the base-file.

General

The base-file needs to be of the ".inp" type, this is an "input file for Abaqus". ".inp-files" are created via Abaqus by, after configuration, creating a "job" and requesting a "write input" for that job. These files can be opened in Abaqus by using "file > import > model". The base-file has to contain all necessary information about the structural model, which includes:

• Mesh defining the structure geometry and discretization.
  • Also the element type needs to be defined.
• Material properties.
• Boundary conditions.
• Surfaces where external loads need to be applied (one surface per ModelPart).
  • Here "Surface" refers to nomenclature of the Abaqus software itself. The name can be found as such in the Abaqus working tree.
• Per surface a pressure load and traction load should be defined (see below).
• Node sets where displacement data will be extracted.
  • Here "Set" refers to nomenclature of the Abaqus software itself. The name can be found as such in the Abaqus working tree. Also element sets exist, but for CoCoNuT the demanded sets need to be a collection of geometrical nodes, hence "node set".
• A Field Output Request requesting output at the node sets (see below).
• A Step definition, which contains solver settings. Currently, the following type of analyses are supported (it is advised to explicitly set them based on this documentation rather than leaving it to Abaqus to fill in a default):
  • Implicit dynamic, application quasi-static
  • Implicit dynamic, application moderate dissipation
  • Implicit dynamic, application transient fidelity
  • Static general
• Additional loads not dependent on the flow solver.

Abaqus models contain parts and those parts are used to create assemblies. The base-file should contain one assembly, which will then be used by the coupling. The assembly, thus, determines the position and orientation that will be used by the coupling software. Also the sets and surfaces required by CoCoNuT should be defined on the assembly level.

Abaqus has a GUI as well as a Python 2 interface (which is also accessible) via the GUI. References to both the Python interface and GUI will be made below.

Setup for Abaqus input (loads)

Per surface in the fluid-structure interface (where loads and displacements need to be exchanged) a "surface" should be created in the assembly. There are multiple possibilities to create these surfaces:

• From the geometry: when the geometry has been defined in Abaqus itself, the geometry faces can easily be selected in the GUI. This method is often the most straightforward, but the Abaqus model should contain the geometry.
• From the mesh: when the geometry is not available (this can for example be the case when a mesh has been imported), a surface can be defined by selecting multiple mesh faces. As a surface typically covers many mesh faces, it is useful there to select the regions "by angle", which uses the angle between mesh faces to determine whether adjacent faces should be selected. This way the surface selection can be extended until a sharp corner is met.
• By converting a "node set" containing all the nodes on the surface and then calling the SurfaceFromNodeSet method which can be found in the make_surface.py file in the extra directory. It is advised to copy this file to the working directory.

An example on the use of SurfaceFromNodeSet (via the Python console in Abaqus or a Python script for Abaqus):

from make_surface import SurfaceFromNodeSet
my_model = mdb.models['Model-1']
my_assembly = my_model.rootAssembly  
my_instance = my_assembly.instances['PART-1-1']
inputSurfaceA = SurfaceFromNodeSet(my_assembly, my_instance, 'NODESET_NAME_A', 'SURFACE_NAME_A')

On these surfaces a "pressure load" and a "surface traction load" need to be specified with a "user-defined" distribution. Loads are assigned to a "step". A step is a part of the simulation to which an analysis type, algorithm settings and incrementation settings are assigned that do not change for the duration of the step. In a typical CoCoNuT case only a single step is defined. Note that the name of the step used for the FSI has to be "Step-1" as this name is hardcoded in GetOutput.cpp. After creation of the step the loads can be assigned. It is required to have the initialConditons=OFF part when using application=TRANSIENT FIDELITY (beware that when application is not specified, transient fidelity is the default). This makes sure that for each time step the accelerations from the previous time step are used. This can be done via the GUI or using Python commands available in Abaqus similar to the following:

from step import *
step1 = my_model.ImplicitDynamicsStep(name='Step-1', previous='Initial', timePeriod=1, nlgeom=ON, maxNumInc=1, haftol=1, initialInc=1, minInc=1, maxInc=1, amplitude=RAMP, noStop=OFF, nohaf=ON, initialConditions=OFF, timeIncrementationMethod=FIXED, application=QUASI_STATIC)
step1.Restart(frequency = 99999, overlay = ON)
my_model.Pressure(name = 'DistributedPressure', createStepName = 'Step-1', distributionType = USER_DEFINED, field = '', magnitude = 1, region=inputSurfaceA)
my_model.SurfaceTraction(name = 'DistributedShear', createStepName = 'Step-1', region = inputSurfaceA, magnitude = 1, traction = GENERAL, directionVector = ((0,0,0), (1,0,0)), distributionType = USER_DEFINED)

The second command enables writing of restart files by Abaqus, which is required for running unsteady cases. This can be done from the GUI when the "Step" module is active in the viewport, by selecting "Output" in the top menu and subsequently "Restart Requests". Frequency should be put on 99999, overlay activated (this spares disk space since only the last increment is kept) and interval on 1 (also see this Abaqus documentation page). Note that the step type "ImplicitDynamicsStep" is an example, it depends on the analysis procedure chosen to run the Abaqus part of the FSI simulation. For a steady simulation this could for example be "StaticStep":

step1 = my_model.StaticStep(name='Step-1', previous='Initial', timePeriod=1.0, initialInc=1, minInc=1e-4, maxNumInc=10, nlgeom=ON, amplitude=RAMP)

The Abaqus wrapper tries to check if the increments comply with the delta_t setting and if needed adjusts it accordingly (notifying the user by raising a warning). The lines in the base-file (.inp) can look similar to this:

*Step, name=Step-1, nlgeom=YES, inc=1
*Dynamic,application=QUASI-STATIC,direct,nohaf,initial=NO
0.0001,0.0001,

It is required to have initial=NO when using the application transient fidelity (default when no application specified). This corresponds to the initialConditons=OFF setting when creating a step using Python. As mentioned earlier, this makes sure that for each time step the accelerations from the previous time step are used. The time step (0.0001) will in this case be replaced by settings found in the JSON file. More information for dynamic cases can be found on this Abaqus documentation page, for static cases on this page.

Input-related settings in JSON file

The name of the surface has to be put as value for the "model_part" key in the interface_input list, but with "_load_points" appended to it. If multiple surfaces are defined, their geometry should match those in the flow solver wrapper counterpart and be listed in the same order.

{
  "interface_input": 
  [
    {
      "model_part": "SURFACE_NAME_A_load_points",
      "variables": ["pressure", "traction"]
    },
    {
      "model_part": "SURFACE_NAME_B_load_points",
      "variables": ["pressure", "traction"]
    }
  ]
}

Setup for Abaqus output (displacements)

After creation of the step, Abaqus needs to be instructed about what to output at the end of a calculation. A "Field Output" has to be generated covering all locations involved in the fluid-structure interface. To do so one must create node sets in the assembly (if this had not been done before) containing all structural nodes of the surfaces, then create a Field Output Request for at least the coordinates and the displacements. This Field Output Request can in the GUI be found as part of the model tree, but below also an example for the Python interface is given. A Field Output Request requests field output (as the name says) to be written to the output database file (.odb).

In the previous section an example was given of how a surface can be created from a node set, but the other way around is also possible, creating a node set from a surface (presuming that this surface was already created):

my_assembly = my_model.rootAssembly
inputSurfaceA = my_assembly.surfaces["SURFACE_NAME_A"]
outputSetA = my_assembly.Set(name='NODESET_NAME_A', nodes=inputSurfaceA.nodes)
my_model.FieldOutputRequest(createStepName='Step-1', frequency=LAST_INCREMENT, name='F-Output-1', region=my_assembly.sets['NODESET_NAME_A'], variables=('COORD', 'U'))

Furthermore, it may be interesting (for post-processing and debugging) to preserve the default Abaqus output and therefore also configure a Field Output and History Output with PRESELECTED variables. This can be done via the GUI or using Python lines similar to the following:

my_model.FieldOutputRequest(createStepName='Step-1', frequency=LAST_INCREMENT, name='F-Output-2', variables=PRESELECT)
my_model.HistoryOutputRequest(createStepName='Step-1', frequency=LAST_INCREMENT, name='H-Output-1', variables=PRESELECT)

Output-related settings in JSON file

The values of the interface_output["model_part"] keys should match the names of the node sets defined in Abaqus, appended with "_nodes". These values are internally used in CoCoNuT to distinguish the different ModelParts. The order defined in the interface_output list should be the same as the interface_input list and match the flow solver wrapper counterpart.

{
  "interface_output": 
  [
    {
      "model_part": "NODESET_NAME_A_nodes",
      "variables": ["displacement"]
    },
    {
      "model_part": "NODESET_NAME_B_nodes",
      "variables": ["displacement"]
    }
  ]
}

Note about choosing ModelParts

The created "surfaces" and "node sets" for load input and displacement output respectively, correspond to ModelParts in the CoCoNuT code, a representation of the data used for the coupling. It is strongly advised to sub-divide to fluid-structure interaction interface intelligently, depending on the geometry. As a rule of thumb it can be said that a surfaces at two sides of a sharp corner should be assigned to a different ModelPart. As the interpolation is based on shortest distance, issues can arise at sharp corners. Those are avoided by having different ModelParts at each side of the corner. Another reason to do this is because the code cannot handle elements with two or more faces being part of the same ModelPart. This situation would occur if the surface contains corners. An example is an airfoil where the suction side and pressure side belong to the same ModelPart: elements at the trailing edge will have (a) face(s) at both the pressure side and suction side. Even when the code would allow this, interpolation mistakes become likely, as a geometrical node or load point on the suction side could have a nearest neighbour on the pressure side, causing that the wrong data is used for interpolation.

Log files

A general event log of the procedure can be found in the working directory, in a file named abaqus.log. For more detailed information on a certain time step, the .msg file written by Abaqus can be consulted. In CoCoNuT these are structured as follows: CSM_TimeA.msg, A being the time step. Typically multiple coupling iterations are done within each time step, so these .msg-files get overwritten by each new coupling iteration in the same time step.

Restarting a calculation

For a restart of a calculation, say at time step B, it is necessary that all the Abaqus simulation files of the previous calculation at time step B are still present. This is in accordance with the save_restart parameter defined in a higher component. Particulary for the Abaqus solver wrapper, it is important that the files CSM_Time0Cpu0SurfaceAFaces.dat, CSM_Time0SurfaceAElements.dat and CSM_Time0SurfaceANodes.dat are still present from previous calculation. The files CSM_Time0.inp and CSM_Restart.inp will be generated during initialization of the restarted calculation. This allows the user to alter some parameters in the input file before restart, e.g. altering output requests, boundary conditions or applying additional loads. Since Abaqus only uses the CSM_Restart.inp (which does not contain any mesh information) and output files of the previous calculation, it is pointless to change the mesh before a restart.

End of the calculation

Unlike for other solvers, CoCoNuT does not keep track of the time it takes to write case files. The reason for this is that Abaqus starts and stops every single coupling iteration, see here and therefore needs data files to be saved every time step in order to continue the calculation in a next coupling iteration or time step. Saving data files is as such seen as inherent to solving the solution step.

Solver coupling convergence

The convergence criterion solver coupling convergence can not be used for the Abaqus solver wrapper.

Version specific documentation

v2023

No major changes.

v2024

Abaqus is now using Python 3.10 instead of Python 2.7.