MultiPhysicsVault/.raw/AbaqusAnalysisUserGuide2/AbaqusAnalysisUserGuide2_077.md

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, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2).
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,” Section 4.1.2, and “Output to the output database,” Section 4.1.3). 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, FREQUENCYTo control the output frequency to the Abaqus/Explicit results file, use the following option:*FILE OUTPUT, NUMBER INTERVALTo control the output frequency to the output database, use the following option:*OUTPUT, FIELD, FREQUENCY

Abaqus/CAE Usage: Step module: Output→Field Output Requests→Create: Frequency

Material options

Any of the material models described in Part V, “Materials,” 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.

Output

Any of the output normally available within a particular procedure is also available during a submodeling analysis (see “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2).

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.

10.2.2 NODE-BASED SUBMODELING

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE

References

• “Submodeling: overview,” Section 10.2.1
• *SUBMODEL
• *BOUNDARY
• Chapter 38, “Submodeling,” of the Abaqus/CAE User’s Guide

Overview

The following types of node-based submodeling are available:

• Same-to-same (e.g., solid-to-solid, shell-to-shell);
• Shell-to-solid; and
• Acoustic-to-structure.

These submodel types support the following nodal-driven variables:

• Displacement,
• Rotation,
• Temperature,
• Pore pressure, and
• Acoustic pressure.

Performing a node-based submodeling analysis

For an overview of submodeling that includes some details common to both node-based and surfacebased submodeling, see “Submodeling: overview,” Section 10.2.1.

Your submodel analysis is driven, either partly or completely, from the results obtained from a global model analysis. The results from the global model are interpolated onto the nodes on the appropriate parts of the boundary of the submodel (see Figure 10.2.2–1). Thus, the response at the boundary of the local region is defined by the solution for the global model. The driven nodes and any loads applied to the local region determine the solution in the submodel.

Different types of node-based submodeling

Three different techniques are available for nodal-based submodeling.

Solid-to-solid submodeling

The linear or nonlinear response of a global solid model can be used to drive the submodel response of a solid submodel. The driven variables can be displacements or temperatures.

text_image

symmetry y x

• submodel boundaries × nodes where global model solution must be stored for interpolation

Figure 10.2.2–1 The global model.

Shell-to-solid submodeling

The linear or nonlinear response of a global shell model can be used to drive the submodel response of a solid submodel. The driven variables are displacements, which are determined from global model displacements and rotations.

Acoustic submodeling

The linear or nonlinear response of a global, structural model can be used to drive the acoustic response of a fluid region of any size if the forces exerted on the structure by the fluid are small. This is often the case for metal structures in air, building interiors, or for sound propagation from a liquid to air. In the case of a liquid and a gas, no special procedures need be followed; the pressure degrees of freedom couple straightforwardly. In the case of a structure driving a fluid, you must ensure that the degrees of freedom to be driven in the submodel exist among the global model results. Several alternatives exist. A thin layer of fluid elements, with the same properties as the submodel fluid, can be added to the global model; this element set and its nodes can then be used to drive the submodel in the usual manner. Alternatively, you can create acoustic interface elements on the surface of the submodel and drive the corresponding nodes with the structural nodes (see “Fully and sequentially coupled acoustic-structural analysis of a muffler,” Section 9.1.1 of the Abaqus Example Problems Guide).

In problems where the fluid exerts large pressures on the structure, the mechanical response of the structure may be of interest. Acoustic-to-structure submodeling can be used in such problems. The submodel in these problems is a part of the structural component of the global model. The acoustic pressure obtained from solving a coupled acoustic-structural global analysis is used to drive the submodel on the surface it shares with the fluid medium. Other boundaries of the submodel may be driven using

the displacements of the structural component of the global model via solid-to-solid submodeling. The acoustic-to-structure submodel analysis solves an uncoupled structural force-displacement problem. The acoustic pressure from the global model is interpolated to the submodel driven nodes. The tributary area and the outward normal associated with the driven node are used to convert the interpolated acoustic pressure to a concentrated load acting at that location (see “Miscellaneous submodeling tests,” Section 3.7.17 of the Abaqus Verification Guide).

Saving the results from the global model

The results from the global analysis must be saved at all nodes required for the interpolation of the driven variables to the boundary of the submodel (see Figure 10.2.2–1). The results (.fil) file or the output database (.odb) file can be used for this purpose.

Saving the results to the results file

In each step of the global model whose solution will be used to drive the submodel, write the nodal results for all driven variables to the results file (see “Output to the data and results files,” Section 4.1.2). These results must be written in the global coordinate system of the model. The submodel can refer only to a global model results file that is from a binary compatible platform.

When the global model is run in Abaqus/Explicit and results file output is requested, the results are written to the selected results (.sel) file; this file needs to be converted into a results (.fil) file using the convert option (see “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2).

Input File Usage: *NODE FILE

(In Abaqus/Standard GLOBAL=NO should not be used on the *NODE FILE option.)

Abaqus/CAE Usage: You cannot write output to the results file in Abaqus/CAE.

Saving the results to the output database

In each step of the global model whose solution will be used to drive the submodel, write the nodal results for all driven variables to the output database in ODB or SIM format (see “Output to the output database,” Section 4.1.3). Unlike the results file, nodal output to the output database is always written in the global directions. The output database can be transferred to any platform since it is binary neutral.

Input File Usage: Use both of the following options:

*OUTPUT, FIELD

*NODE OUTPUT

Abaqus/CAE Usage: Step module: Output→Field Output Requests→Create

Saving results with higher precision

By default, the nodal output to the output database is written using single precision, which may not be sufficient for certain classes of problems; for example, submodels undergoing large rigid body motions (consider also surface-based submodeling in these cases—see “Surface-based submodeling,”

Section 10.2.3). For such analyses request the nodal output to the fullest possible precision (see “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2).

Input File Usage: abaqus job=global_model_input_file output_precision=full

Abaqus/CAE Usage: Job module: Create Job: Precision: Nodal output precision: Full

Saving results from a global model with a physical time scale

If the global analysis in Abaqus/Standard involves a physical time scale and the results file is to be used in the submodel analysis, request that the results file output be written at the beginning of the step (the zero increment) for all steps in the global analysis (see “Output,” Section 4.1.1). Abaqus will then have the complete solution history (including the solution state at the beginning of a step) from which a submodel may be driven. If the zero increment results are not requested, incorrect results will be obtained if the step time in the submodel is less than the step time of the first increment on the results file. Instead of interpolating between the results at the start of the step and the results of the first increment on the results file, Abaqus will simply use the results of the first increment as long as the submodel step time is less than the step time of the first increment on the results file. The zero increment request is not required in Abaqus/Explicit, because the results are always written to the results file at the beginning of each step. Similarly, the results will always be correctly interpolated when using the output database to transfer the results from the global model to the submodel, because the zero increment is always written to the output database.

Input File Usage: *FILE FORMAT, ZERO INCREMENT

Abaqus/CAE Usage: You cannot write output to the results file in Abaqus/CAE.

Referring to the global model results from the submodel analysis

You must define the source of the global solution results. Provide the name of the global results file or output database file (in ODB or SIM format); the file extension is optional. If the file extension is omitted, Abaqus will use in order, the results file, the ODB output database file, or the SIM database file.

Input File Usage: abaqus job=submodel_input_file globalmodel=global_results_file or global_output_database or sim_database_file

Abaqus/CAE Usage: Any module: Model→Edit Attributes→submodel: Submodel: Read data from job: global_results_file or global_output_database Reading data from a SIM database file is not supported in Abaqus/CAE.

Specifying the driven nodes in the submodel

Specifying the driven nodes does not activate the driven variables: they must be activated by specifying the appropriate submodel boundary conditions.

All nodes of the submodel where variables will be driven in any step (see Figure 10.2.2–2) must be specified as driven nodes since the list of nodes cannot be extended subsequent to its initial definition (even at restart). However, variables at the nodes given do not have to be driven in all steps: the choice of which variables are driven in a particular step is made as part of a submodel boundary condition definition, as discussed later.

radar

x	y	boundary nodes of the submodel driven by global model solution
0	0	0
1	1	1
2	2	2
3	3	3
4	4	4
5	5	5
6	6	6
7	7	7
8	8	8
9	9	9
10	10	10
11	11	11
12	12	12
13	13	13
14	14	14
15	15	15
16	16	16
17	17	17
18	18	18
19	19	19
20	20	20
21	21	21
22	22	22
23	23	23
24	24	24
25	25	25
26	26	26
27	27	27
28	28	28
29	29	29
30	30	30
31	31	31
32	32	32
33	33	33
34	34	34
35	35	35
36	36	36
37	37	37
38	38	38
39	39	39
40	40	40
41	41	41
42	42	42
43	43	43
44	44	44
45	45	45
46	46	46
47	47	47
48	48	48
49	49	49
50	50	50
51	51	51
52	52	52
53	53	53
54	54	54
55	55	55
56	56	56
57	57	57
58	58	58
59	59	59
60	60	60
61	61	61
62	62	62
63	63	63
64	64	64
65	65	65
66	66	66
67	67	67
68	68	68
69	69	69
70	70	70
71	71	71
72	72	72
73	73	73
74	74	74
75	75	75
76	76	76
77	77	77
78	78	78
79	79	79
80	80	80
81	81	81
82	82	82
83	83	83
84	84	84
85	85	85
86	86	86
87	87	87
88	88	88
89	89	89
90	90	90
91	91	91
92	92	92
93	93	93
94	94	94
95	95	95
96	96	96
97	97	97
98	98	98
99	99	99
100	100	100

Figure 10.2.2–2 The magnified submodel.

Input File Usage:

*SUBMODEL

list of nodes or node set labels or, for acoustic-to-structure submodeling, the name of an element-based structural surface

The *SUBMODEL option must be included in the model definition portion of the input file for the submodel analysis. Multiple *SUBMODEL options are allowed; however, in this case you must ensure that the driven nodes specified on the data line of one option are separate and distinct from the nodes specified on the data lines of all the other options.

Abaqus/CAE Usage:

Load module: Create Boundary Condition: choose Other for the Category and Submodel for the Types for Selected Step: select region

Specifying the driven nodes in shell-to-solid submodeling

In shell-to-solid submodeling, the submodel is made up of solid elements and replaces a region where conventional shell elements are used in the global model. In this case Abaqus expects that all the driven nodes on the submodel belong to solid elements and are driven from a global model region that is entirely made up of shell elements. The boundary where the submodel is driven is a set of surfaces in the submodel but is a set of lines in the shell reference surface in the global model, as shown in Figure 10.2.2–3. The dashed line on the shell model is replaced by the shaded surfaces of the solid element submodel.

text_image

A B C

a) Shell global model with submodel boundaries

text_image

A B C

A, B, C - shell reference surface

• driven nodes

b) Magnified solid element submodel

Figure 10.2.2–3 Shell-to-solid submodeling.

Whenever shell-to-solid submodeling is used, you must define the maximum shell thickness in the global model, given in the units used for the models. If a shell offset is defined in the global model, the shell thickness must be set equal to twice the maximum distance from the top or bottom shell surface to the shell reference surface.

Input File Usage: *SUBMODEL, SHELL TO SOLID, SHELL THICKNESS=thickness

If more than one *SUBMODEL option is used, the SHELL TO SOLID parameter must be included on every option.

Abaqus/CAE Usage: Any module: Model→Edit Attributes→submodel: Submodel: Shell global model drives a solid submodel

Load module: Create Boundary Condition: choose Other for the Category and Submodel for the Types for Selected Step:

select region: Shell thickness: thickness

Specifying the driven nodes in acoustic-to-structure submodeling

The global analysis for acoustic-to-structure submodeling problems is performed as a coupled acousticstructural analysis. The acoustic nodal pressures from the global analysis must be written to the results file for the acoustic mesh in contact with the structural surface of interest. In the submodel analysis acoustic pressures from the global analysis drive the user-specified structural surface of interest. The driven nodes for the submodel are the nodes lying on the specified surface. Only element-based surfaces are allowed in acoustic-to-structure submodeling.

Input File Usage: *SUBMODEL, ACOUSTIC TO STRUCTURE, ABSOLUTE EXTERIOR TOLERANCE=value

Abaqus/CAE Usage: Acoustic-to-structure submodeling is not supported in Abaqus/CAE.

Specifying driven nodes for shells with acoustic pressures on both sides

In certain problems the acoustic pressure may act on both sides of a shell structure. Figure 10.2.2–4 shows a section of a global model consisting of a shell structure that is sandwiched between two acoustic media.

text_image

acoustic region 1 SPOS shell structure SNEG y x ELSET = Acoustic_SPOS ELSET = Acoustic_SNEG acoustic region 2

Figure 10.2.2–4 A cross-section of the acoustic-to-structure global model with acoustic regions on both sides of the shell.

Separate element sets consisting of acoustic elements on the positive and negative sides of the shell are defined, respectively. The nodal pressures for nodes attached to elements in these sets are written to the selected results file. Figure 10.2.2–5 shows the submodel that consists only of the refined shell structure.

text_image

surface Shell_SPOS driven node shell structure surface Shell_SNEG y x

Figure 10.2.2–5 The acoustic-to-structure submodel with acoustic pressure on both sides of the shell.

Two separate surfaces are defined on the SPOS and SNEG sides, respectively. To apply the acoustic pressure from the global analysis on each side of the shell correctly, you must specify the surface name along with the corresponding acoustic element set.

Input File Usage: *SUBMODEL, ACOUSTIC TO STRUCTURE, GLOBAL
ELSET=Acoustic_SPOS
Shell_SPOS
*SUBMODEL, ACOUSTIC TO STRUCTURE, GLOBAL
ELSET=Acoustic_SNEG
Shell_SNEG 

Abaqus/CAE Usage: Acoustic-to-structure submodeling is not supported in Abaqus/CAE.

Defining geometric tolerances

A geometric tolerance is used to define how far a boundary node in the submodel can lie outside the exterior surface of the global model, as that surface is interpolated in the global, undeformed finite element model. By default, nodes in the submodel must lie within a distance calculated by multiplying the average element size in the global model by 0.05. You can change the tolerance, which is useful in cases where submodel driven nodes lie to a greater extent outside the global model exterior surface. Tolerances larger than this default value, however, may result in significantly greater computation times and lower accuracy in the driven solution for driven nodes significantly outside the global model exterior surface.

You can define the geometric tolerance as a fraction of the size of the average element in the global model or as an absolute distance in the length units chosen for the model. If both tolerances are defined, Abaqus uses the tighter tolerance.

Input File Usage: Use the following option to define the geometric tolerance as an absolute distance:
*SUBMODEL, ABSOLUTE EXTERIOR TOLERANCE=tolerance
Use the following option to define the geometric tolerance as a fraction of the size of the average element in the global model:
*SUBMODEL, EXTERIOR TOLERANCE=tolerance
Abaqus/CAE Usage: Load module: Create Boundary Condition: choose Other for the Category and Submodel for the Types for Selected Step: select region: Exterior tolerance: absolute: or relative: tolerance 

The exterior tolerance in solid-to-solid submodeling

The exterior tolerance for a solid-to-solid submodel analysis is indicated by the shaded region in Figure 10.2.2–6. If the distance between the driven nodes and the free surface of the global model falls within the specified tolerance, the solution variables from the global model are extrapolated to the submodel.

The exterior tolerance in shell-to-shell submodeling

In a shell-to-shell submodel analysis Abaqus checks whether the driven nodes of the submodel lie sufficiently close to the reference surface of the shell elements in the global model. To simplify calculations, the closest point in the global model is calculated as the intersection of a line drawn