About Submodeling

The submodeling technique:

  • 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 drive a local part of the model by nodal results, such as displacements (see Node-Based Submodeling Using the Submodel Interface later in this section), or by the element stress results (see Surface-Based Submodeling later in this section) from the global mesh;

  • 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).

This page discusses:

See Also
Node-Based Submodeling
Surface-Based Submodeling
In Other Guides
Output to the Output Database
*SUBMODEL
Submodeling

Products Abaqus/Standard Abaqus/Explicit Abaqus/CAE

Introduction

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.

Input File Usage

SUBMODEL, TYPE=NODE

Abaqus/CAE Usage

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.

Input File Usage

FIELD IMPORT, SUBMODEL
EXTERNAL FIELD

Abaqus/CAE Usage

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

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.

Input File Usage

SUBMODEL, TYPE=SURFACE

Abaqus/CAE Usage

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
  • Surface-based (stress) technique: output database (.odb) file or SIM database (.sim) file
  • Beam-to-solid technique: 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.

Input File Usage

SUBMODEL, GLOBAL ELSET=name

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).

Input File Usage

FIELD IMPORT, SUBMODEL
EXTERNAL FIELD
 , , , , global_elset_name, ,

Abaqus/CAE Usage

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:

  1. 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).

  2. 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:

NODE FILE, FREQUENCY

To control the output frequency to the Abaqus/Explicit results file, use the following option:

FILE OUTPUT, NUMBER INTERVAL

To control the output frequency to the output database, use the following option:

OUTPUT, FIELD, FREQUENCY

Abaqus/CAE Usage

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.