Product: ABAQUS/Explicit
“Preparing an ABAQUS analysis for co-simulation,” Section 13.1.2
ABAQUS User's Guide for Crash Safety Simulation Using ABAQUS/Explicit and MADYMO
MADYMO Reference Manual
The co-simulation technique can be used for crash safety simulations performed in conjunction with the occupant simulation program MADYMO. Co-simulation using ABAQUS/Explicit and MADYMO is available as an add-on analysis capability.
For co-simulation with MADYMO the start of the co-simulation event must be defined at the beginning of an ABAQUS/Explicit step. When that step is reached during the analysis, ABAQUS launches and establishes a communication mechanism with the MADYMO solver. The interface regions defined in the ABAQUS model are conveyed to the MADYMO solver.
In the MADYMO model you can group the interface regions from the ABAQUS model suitably for use in contact definitions with the interface regions in the MADYMO model. The contact condition between the interface regions of the two models is enforced by MADYMO. Co-simulation with ellipsoidal, faceted, and finite element models in MADYMO is supported.
Both programs advance the coupled analysis by using identical time incrementation and exchanging the necessary data at every increment. The time increment is computed to be the minimum of the values preferred by the two programs at any stage of the co-simulation.
When the unit system used in creating the ABAQUS model is not the same as that used in creating the MADYMO model, conversion factors can be specified in the ABAQUS model (see “Preparing an ABAQUS analysis for co-simulation,” Section 13.1.2).
For a detailed description of the co-simulation with MADYMO capability, see the ABAQUS User's Guide for Crash Safety Simulation Using ABAQUS/Explicit and MADYMO.
An integer identifier can be assigned to each interface region in the ABAQUS model. These identifiers, and not the surface names used in defining the interface region, are exported to MADYMO. Along with the identifiers, the element numbers and the node numbers used in the ABAQUS model are exported to MADYMO. You can define groups in the MADYMO model by selecting the desired region identifiers, the node numbers, and/or the element numbers from the ABAQUS model.
| Input File Usage: | Use the following options to define a co-simulation region in an ABAQUS model using an integer identifier: |
*CO-SIMULATION, PROGRAM=MADYMO *CO-SIMULATION REGION, REGION ID=n surface_A, surface_B, Repeat the *CO-SIMULATION REGION option to define interface regions with different integer identifiers. |
For co-simulation with MADYMO the list of quantities to be exported and imported over a co-simulation region is predetermined by the MADYMO programming interface. At run time ABAQUS/Explicit exports the coordinates and imports the concentrated nodal forces for the nodes on the interface regions in the ABAQUS model. At the beginning of the co-simulation analysis ABAQUS/Explicit also exports the discrete nodal masses and an effective bulk modulus, a thickness averaged over all the elements underlying the various surfaces for a co-simulation region in the ABAQUS model.
| Input File Usage: | Use the following options to identify the surfaces forming a co-simulation region (no quantity identifiers are listed for the solution quantities to be exported or imported). ABAQUS automatically selects the solution quantities for exchange. |
*CO-SIMULATION, PROGRAM=MADYMO *CO-SIMULATION REGION surface_A, surface_B, |
ABAQUS does not require that the analysis be run with a particular unit system. However, if you have created the ABAQUS model with a unit system that is different than the unit system for the MADYMO model, ABAQUS provides a method for conversion between the unit systems.
In the ABAQUS model you can specify a set of conversion factors for the basic units of mass, length, and time. If a solution quantity with the units of length is exported, ABAQUS multiplies this quantity by the length unit conversion factor prior to exporting the value to the third-party program. Similarly, if a solution quantity with the units of length is imported, ABAQUS divides this quantity from the third-party program by the length unit conversion factor prior to using the solution quantity in the ABAQUS model. The conversion factors are constructed for the various solution quantities that are exchanged based on the conversion factors for the basic units.
| Input File Usage: | Use the following option to specify unit conversion factors when there is a mismatch in unit systems between the ABAQUS/Explicit model and the MADYMO model: |
*CO-SIMULATION, PROGRAM=MADYMO mass unit conversion factor, length unit conversion factor, time unit conversion factor |
As described in “Preparing an ABAQUS analysis for co-simulation,” Section 13.1.2, you must identify the interface regions of the ABAQUS model. For each interface region ABAQUS exports the integer identifier, the coordinates of the nodes in the interface region and their user-defined numbers, and the connectivity of the facets forming the interface region and their user-defined underlying element numbers to MADYMO. You need to modify the MADYMO model to use these data from ABAQUS to define contact conditions with the corresponding interface regions of the MADYMO model. A guideline for modifying the MADYMO model to define a contact condition between the interface regions of the two models is provided in the ABAQUS User's Guide for Crash Safety Simulation Using ABAQUS/Explicit and MADYMO.
All contact types in MADYMO can be used (elastic and penalty-based) except kinematic contact. Furthermore, damping can be included in the contact definition. You should check the reprint file from MADYMO between the lines COUPLING INTERFACE and END COUPLING INTERFACE to make sure that the ABAQUS interface region data are transferred correctly.
The coupled job is run interactively using the ABAQUS execution procedure with ABAQUS/Explicit running either in serial or parallel mode. For more information on using the madymo command line option, see “Execution procedure for ABAQUS/Standard and ABAQUS/Explicit,” Section 3.2.2, and the ABAQUS User's Guide for Crash Safety Simulation Using ABAQUS/Explicit and MADYMO.
You need to specify the location of the MADYMO installation by setting madymo_home to $MADYMO_HOME in the abaqus_v6.env file. For example:
madymo_home="/p/third_party_software/Madymo/madymo_62"
Prior to launching the coupled job, the MADYMO model must be converted from the .xml file format to the .saf file format using the bsaf executable in the MADYMO installation. For more information, see the ABAQUS User's Guide for Crash Safety Simulation Using ABAQUS/Explicit and MADYMO.
Co-simulation with MADYMO is subject to the following limitations:
The co-simulation functionality between MADYMO and ABAQUS/Explicit is currently limited to the HP-UX/Itanium platform.
A MADYMO model is always three-dimensional. The corresponding ABAQUS model must also be three-dimensional.
The surfaces used in defining co-simulation regions in the ABAQUS model must be such that no nodes are shared with each other.
MADYMO is always run serially even when ABAQUS/Explicit is run in parallel, which can potentially reduce the CPU peformance scale factor in parallel.
The ABAQUS/Explicit analysis will continue after the co-simulation event until the end of the steps defined in the ABAQUS model. You can monitor the ABAQUS job by inspecting the status file, which will print a message when the co-simulation event ends. At that time check the reprint file from MADYMO to see if MADYMO has ended prematurely with an error message. If so, you may want to terminate the ABAQUS process manually.
Due to the necessary communication sequence between MADYMO and ABAQUS/Explicit, the stable time increment in ABAQUS/Explicit is limited to element-wise stability values and is likely to be smaller than a value computed for an ABAQUS/Explicit analysis without co-simulation.
The following software is required:
ABAQUS/Explicit Version 6.6. The installation should have the necessary permissions to run a co-simulation with MADYMO. For contact information, refer to http://www.abaqus.com.
MADYMO Version 6.2. MADYMO is distributed and licensed by TNO MADYMO BV. The installation should have the necessary permissions to run a co-simulation with ABAQUS/Explicit. For contact information, refer to http://www.automotive.tno.nl.