is used to study a local part of a model with a refined mesh based on interpolation of
the solution from an initial (undeformed), relatively coarse, global model;
is most useful when it is necessary to obtain an accurate, detailed solution in a local
region and the detailed modeling of that local region has negligible effect on the overall
solution;
can be used to analyze an acoustic model driven by displacements from a structural,
global model when the acoustic fluid has negligible effect on the structural solution;
can be used for the analysis of a structure driven by acoustic pressures from an acoustic
or coupled acoustic-structural, global model;
can be used to drive a surface representing a beam of a submodel driven by the
displacement and rotations of a structural beam element in the global model;
can use a combination of Abaqus/Explicit and Abaqus/Standard procedures;
can use a combination of linear and nonlinear procedures; and
cannot be used to drive a time-domain analysis with the results from a frequency-domain
analysis (or vice versa).
The submodeling technique allows you to follow up a simulation with a detailed study of one
or more local regions of interest, with the results from the original simulation providing
the boundary conditions for these local simulations. The original model is referred to as
the “global” model and a subsequent detailed model is referred to as a “local” model or a
“submodel.” You identify the regions to investigate with submodeling during postprocessing
of the global model. A submodel simulation typically goes through approximately the same
configuration and stress evolution in the submodel region as the global model but with more
detailed and accurate resolution of the results. The driven variables can be degrees of
freedom at the nodes in the node-based technique, or they can be components of the stress
tensor at the integration points of element faces in the surface-based technique.
Submodeling is often much more efficient than using a globally refined model. The accuracy
of submodel results relies on sufficient accuracy of the global results that drive results
at the submodel boundary “cuts.” Submodeling leverages Saint-Venant’s principle that the
difference between the effects of two different but statically equivalent loads becomes very
small at sufficiently large distances from the loading. Judgment is required to position the
submodel cuts far enough away from locations where you desire greater accuracy.
Submodeling Techniques
Submodeling can be applied quite generally in Abaqus. The material response defined for the submodel might be different from that defined for
the global model. Both the global model and the submodel can have nonlinear response. See
Shell-to-solid submodeling and shell-to-solid coupling of a pipe joint for an example
application of the submodeling technique.
Submodeling is classified first according to which of three basic techniques is used. The
most common, and more general technique, is node-based submodeling, which uses a nodal
results field (including displacement, temperature, or pressure degrees of freedom) to
interpolate global model results onto the submodel nodes. The alternative surface-based
technique uses the stress field to interpolate global model results onto the submodel
integration points on the driven element-based surface facets. The third technique is
beam-to-solid submodeling, which can be used only when a submodel uses solid elements where
the global model used beam elements.
Some subtopics in this section do not discuss beam-to-solid submodeling. For more
information about the specialized user interface for beam-to-solid submodeling, see Beam-to-Solid Submodeling.
You can choose either the node-based or surface-based technique or a combination of the two
in your submodel. You cannot combine beam-to-surface submodeling with any other
technique.
You should consider the following factors in deciding whether to use the node-based or
surface based technique:
Whether you are performing solid-to-solid submodeling in a general static analysis in
Abaqus/Standard:
Surface-based submodeling is available only for solid models and static analyses.
For all other procedures use the node-based technique.
Whether the global model and submodel differ significantly in their average stiffness
in the region of the submodel:
When the stiffness of the models is comparable, node-based submodeling of
displacements will provide comparable results to the surface-based technique with a
lesser likelihood of numerical issues associated with rigid-body modes.
When the stiffness of the models differs and the global model is exposed primarily
to a load-controlled environment, the surface-based technique will generally provide
more accurate stress results. Stiffness differences may arise due to additional
detail in the submodel, such as explicit modeling of a fillet or a hole. In other
cases stiffness changes may result from minor geometry changes for which a
reanalysis of the global model is not warranted.
Whether your model is subjected to large deformations or rotations:
Node-based submodeling of displacements will result in more accurate transmission
of large deformation and rotation to the submodel.
Whether the displacement response of the global model corresponds to the displacement
response of the submodel:
When the displacements in the global model correspond closely with the expected
displacements in the submodel, node-based submodeling is generally preferable.
Surface-based submodeling should be used when the submodel displacement response is
expected to differ from the global model response. This situation can occur when
thermal strains are modeled and the temperature history of the submodel differs from
that of the global model; for example, when heat transfer submodeling is performed
as part of a sequential thermal-structural analysis.
The stiffness of the structure:
Surface-based submodeling may provide more accurate results for very stiff
structures. When the structure is so stiff that only a small component of the global
model displacement field contributes to the stress response, numerical roundoff in
the displacement results can become significant; for example, when the global model
displacement is dominated by a rigid-body motion component.
The type of output you are interested in from the submodel:
Node-based submodeling of displacements will result in more accurate transmission
of a displacement field.
Surface-based submodeling will result in more accurate transmission of a stress
field, and determination of reaction forces in the submodel.
Node-Based Submodeling
Two techniques are available for node-based submodeling: one technique uses the submodel
interface and the other technique uses field import.
Node-Based Submodeling Using the Submodel Interface
Node-based submodeling using the submodel interface is a more general technique than
surface-based submodeling. It supports a variety of element type combinations and
procedures in both Abaqus/Explicit and Abaqus/Standard.
Load module: Create Boundary Condition: choose Other for the Category and Submodel for the Types for Selected Step: Driving region: Specify
Element Types Supported
You can use different element types in the submodel than those used to model the
corresponding region in the global model.
The following types of submodeling are provided for the node-based approach
(global-to-submodel):
Two-dimensional models:
Solid-to-solid
Acoustic-to-structure
Three-dimensional models:
Solid-to-solid
Shell-to-shell
Membrane-to-membrane
Shell-to-solid
Acoustic-to-structure
A global or submodel region that is meshed with continuum shell elements constitutes a
three-dimensional solid region in the submodeling technique. Hence, the use of the
submodeling technique for models involving continuum shell elements is the same as with
models involving continuum solid elements such as
C3D8R or
C3D6.
Procedures Supported
Both the global model and the submodel can have nonlinear response and can be analyzed
for any sequence of analysis procedures. These procedures do not have to be the same for
both models. For example, the linear or nonlinear dynamic response of the global model
can be used to drive the static, nonlinear response of the submodel on the grounds that
the submodel is too small for dynamic effects to be significant in that local region.
The global procedure can be performed in Abaqus/Standard to drive a submodeling procedure in Abaqus/Explicit and vice versa. For example, a static analysis performed in Abaqus/Standard can drive a quasi-static Abaqus/Explicit analysis in the submodel. The step time used in these analyses can be different; the
time variable of the amplitude functions generated at the driven nodes can be scaled to
the step time used in the submodel.
Your submodel cannot refer to a global model step that includes multiple load cases
(see Multiple Load Case Analysis). You must perform the global analysis
with a single load definition for the step that will drive the submodel.
Node-Based Submodeling Using the Field Import Interface
Node-based submodeling using field import is an alternative approach for submodeling.
Instead of using the submodel interface as described above, the field import interface is
used to provide the necessary information. For each part of information that you provide
using the submodel interface, an alternate way to provide the same part of information
exists in the field import interface. For example, the global model name is provided as a
parameter, the global element set is the source element set, and separate boundary
conditions are not required. Node-based submodeling using field import allows for a large
variety in the choice of driven variables in both Abaqus/Explicit and Abaqus/Standard. This approach reduces the preprocessor memory requirements, which is beneficial in
very large models.
Node-based submodeling using the field import interface is not supported in Abaqus/CAE.
Element Types Supported
You can use different element types than those used in the submodel to model the
corresponding region in the global model.
The following types of submodeling for three-dimensional models are provided for the
node-based approach (global-to-submodel):
Solid-to-solid
Shell-to-shell
Membrane-to-membrane
Procedures Supported
Only time-based analysis procedures are supported using this method (see General Capability for Importing External Fields). Submodeling using this method cannot
be performed in a perturbation step.
Surface-Based Submodeling
Surface-based submodeling is provided as a complement to the node-based technique, enabling
you to drive the submodel with stresses from the global model.
Load module: Create Load: choose Mechanical for the Category and Submodel for the Types for Selected Step: Driving region: Specify
Element Types Supported
The following types of submodeling are provided for the surface-based approach
(global-to-submodel):
Two-dimensional models:
Solid-to-solid
Three-dimensional models:
Solid-to-solid
You can use different element types in the submodel than those used to model the
corresponding region in the global model. Continuum elements supported for the static
analysis procedure are supported for surface-based submodeling, with the following
exceptions:
Cylindrical elements are not supported.
Continuum shell elements are not supported.
Continuum solid elements with composite sections are not supported.
Procedures Supported
The surface-based technique is implemented only for static analysis in Abaqus/Standard.
Your submodel cannot refer to a global model step that includes multiple load cases (see
Multiple Load Case Analysis). You must perform the global analysis with a
single load definition for the step that will drive the submodel.
Beam-to-Solid Submodeling
Beam-to-solid submodeling (Beam-to-Solid Submodeling) imposes
displacement and rotations obtained from beam elements in a global model onto a surface of a
solid element mesh of the beam in submodel.
Element Types Supported
Beam-to-solid submodeling uses solid elements in the submodel. Beam-to-solid submodeling
does not support two-dimensional or axisymmetric analysis.
Procedures Supported
Both the global model and the submodel can have nonlinear response and can be analyzed
for any sequence of analysis procedures. These procedures do not have to be the same for
both models. For example, the linear or nonlinear dynamic response of the global model can
be used to drive the static, nonlinear response of the submodel on the grounds that the
submodel is too small for dynamic effects to be significant in that local region. You
cannot use beam-to-solid submodeling in Abaqus/Explicit analyses. Structural beam elements do not have temperature degrees of freedom;
therefore, beam-to-solid submodeling does not support temperature degrees of freedom.
Your submodel cannot refer to a global model step that includes multiple load cases (see
Multiple Load Case Analysis). You must perform the global analysis with a
single load definition for the step that will drive the submodel.
Performing a Submodeling Analysis
A submodeling analysis consists of:
running a global analysis and saving the results in the vicinity of the submodel
boundary;
defining the total set of driven nodes or driven surfaces in the submodel;
defining the time variation of the driven variables in the submodel analysis by
specifying the actual nodes and degrees of freedom or element-based surfaces to be
driven in each step; and
running the submodel analysis using the “driven variables” to drive the solution.
Linking the Global Model and the Submodel
The submodel is run as a separate analysis from the global analysis. The only link
between the submodel and the global model is the transfer of the time-dependent values of
variables saved in the global analysis to the relevant boundary nodes of the submodel or
to the relevant boundary surfaces. The location where the results from the global model
are saved depends on the technique used:
Node-based using the submodel interface: results (.fil) file,
output database (.odb) file, or
SIM database (.sim) file
Node-based using the field import interface: SIM
database (.sim) file
The transfer is achieved by then reading these results into the submodel analysis. If the
global model is defined in terms of an assembly of part instances, the part
(.prt) file from the global model is required for the submodel
analysis.
Since the submodel is a separate analysis, submodeling can be used to any number of
levels; a submodel can be used as the global model for a subsequent submodel.
Accuracy
The global model in a submodeling analysis must define the submodel boundary response
with sufficient accuracy. It is your responsibility to ensure that any particular use of
the submodeling technique provides physically meaningful results. In general, the solution
at the boundary of the submodel must not be altered significantly by the different local
modeling. There is no built-in check of this criterion in Abaqus; it is a matter of judgment on your part. In general, accuracy can be checked by
comparing contour plots of important variables near the boundaries of the submodeled
region.
Specifying the Global Elements Used to Drive the Submodel
By default, the global model in the vicinity of the submodel is searched for elements that
encompass the locations of driven nodes or driven surfaces' faces; the submodel is then
driven by the response of these elements. In some cases more than one element can encompass
the location of a driven node. For example, adjacent bodies in the global model may have
temporarily coincident nodes or surfaces, as depicted in Figure 1.
Figure 1. A global model with coincident surfaces in the area of the local model's driven
nodes.
In this case the location of the driven node in the corresponding global model is touching
both element A and element C; however, only the results from element A should drive the node
in the submodel.
To preclude certain elements from driving the submodel, you have the option of specifying a
global element set to limit the search to an appropriate subset of the global model.
Using the Submodel Interface
You provide the global element set to drive the submodel when using the submodel
interface.
If the global model is defined in terms of an assembly of part instances, give the
complete name—including the assembly and part instance names—when specifying the global
element set. For example, an element set named top in
part instance I-1 of assembly
Assembly-1 must be referred to by
Assembly-1.I-1.top.
If the submodel is not defined in terms of an assembly of part instances, the dots
in the global element set name must be replaced by underscores:
Assembly-1_I-1_top.
If the global element set is defined at the assembly level, you may provide the
element set name without qualifying it with the assembly name in a submodel
analysis.
Abaqus/CAE Usage
Load module: Create Boundary Condition: choose Other for the Category and Submodel for the Types for Selected Step: Driving region: Specify
Using the Field Import Interface
You provide the global element set as the source element set for the external field when
using field import to drive the submodel analysis (available only for node-based
submodeling).
Node-based submodeling using the field import interface is not supported in Abaqus/CAE.
Minimizing File Sizes
The size of the results file or the output database can be minimized for a submodeling
analysis by requesting output for only those global nodes and global elements that are used
to drive the submodel. To determine which global nodes and/or elements are used to drive the
submodel, do the following:
Run a data check analysis on the global model with any combination of results file or
output database file output requests. A data check analysis is performed by using the
datacheck parameter in the command for running Abaqus (Abaqus/Standard and Abaqus/Explicit Execution).
Run a data check analysis on the submodel.
A listing of the global nodes and/or elements that will be used to drive the submodel is
output to the data file during the submodeling data check analysis.
Frequency of Output
Pay special attention to the frequency at which you request output in the global model (see Output to the Data and Results Files and Output to the Output Database). It is possible to define the results file output or
nodal and element output to the output database file such that the information is written at
different frequencies for different nodes and elements, although that should not be done for
nodes and elements involved in the interpolation to define values at driven variables since
Abaqus will take values at the coarsest frequency only. To avoid this problem, write the nodal
and elemental output to the output database or the results file using the same frequency for
all nodes and elements involved in the interpolation and choose a frequency that will allow
the history in the submodel to be reproduced accurately.
Input File Usage
To control the output frequency to the Abaqus/Standard results file, use the following option:
Step module: OutputField Output RequestsCreate: Frequency
Material Options
Any of the material models described in Abaqus Materials Guide can be used in the global and
submodel analyses. The material response defined for the submodel may be different from that
defined for the global model.
Elements
The dimensionality of the submodel must be the same as that of the global model: both
models must be either two-dimensional or three-dimensional. The following limitations apply:
The boundary nodes of the submodel must lie within regions of the global model where
Abaqus is able to perform spatial interpolation to define the values of the driven
variables. Therefore, they must lie within (or, as allowed by the exterior tolerance,
near to) two- or three-dimensional geometrically defined elements in the global model.
Such geometrically defined elements are:
first- or second-order triangles or quadrilaterals in two dimensions;
first- or second-order triangular or quadrilateral shells; and
first- or second-order tetrahedra, wedges, or bricks in three dimensions.
The boundary nodes cannot lie in regions of the global model where there are only
one-dimensional elements (beams, trusses, links, axisymmetric shells) since Abaqus does not provide the necessary interpolation of results for such elements.
The boundary nodes cannot lie in regions of the global model where there are only user
elements, substructures, springs, dashpots, cohesive elements, etc. since those element
types do not allow for geometric interpolation.
The boundary nodes cannot lie in regions of the global model where there are only
axisymmetric solid elements with nonlinear, asymmetric deformation
(CAXA elements). The submodeling
capability is currently not supported for these elements.
The reference node associated with generalized plane strain elements
(CPEG) cannot be used as a driven boundary
node in a submodeling analysis.
As described above, nodal output requests to the results file or output database file must
be used in the global analysis to save the values of the driven variables at the submodel
boundary.
