add documents
This commit is contained in:
김경종
@@ -0,0 +1,368 @@
|
||||
<!-- source-page: 781 -->
|
||||
|
||||
analysis step—followed by extraction of the eigenmodes of the preloaded structure, then a step of 5 seconds of modal dynamic response analysis:
|
||||
|
||||
```txt
|
||||
*STEP
|
||||
** Apply preload
|
||||
*STATIC
|
||||
0.1, 1.0
|
||||
...
|
||||
** Write out results for nodes needed to
|
||||
** interpolate to the submodel's boundary
|
||||
*NODE FILE, NSET=DETAIL
|
||||
U
|
||||
*END STEP
|
||||
*STEP
|
||||
** Calculate modes and frequencies
|
||||
*FREQUENCY
|
||||
...
|
||||
** The *NODE FILE option is repeated because
|
||||
** this is the first linear perturbation step
|
||||
*NODE FILE, NSET=DETAIL
|
||||
U
|
||||
*END STEP
|
||||
*STEP
|
||||
** Dynamic response of preloaded system
|
||||
*MODAL DYNAMIC
|
||||
0.01, 5.0
|
||||
...
|
||||
*END STEP
|
||||
```
|
||||
|
||||
We wish to study the local, possibly nonlinear, response of a part of this model that is so small that we do not need to model dynamic effects locally and can, thus, perform two steps of static analysis:
|
||||
|
||||
```txt
|
||||
** Define submodel boundary (driven nodes)
|
||||
*SUBMODEL
|
||||
PERIM
|
||||
*STEP
|
||||
** Preload
|
||||
*STATIC
|
||||
0.1, 1.0
|
||||
*BOUNDARY, SUBMODEL, STEP=1
|
||||
...
|
||||
*END STEP
|
||||
*STEP
|
||||
```
|
||||
|
||||
<!-- source-page: 782 -->
|
||||
|
||||
```csv
|
||||
** Local static response to global dynamic step
|
||||
*STATIC
|
||||
0.01, 5.0
|
||||
*BOUNDARY, SUBMODEL, STEP=3
|
||||
...
|
||||
*END STEP
|
||||
```
|
||||
|
||||
It is perfectly acceptable that the submodel analysis requests general, possibly nonlinear, analysis for both steps, while in the global analysis the dynamic step was a linear perturbation step (modal dynamics is always a linear perturbation analysis). It is your responsibility to judge that this use of the submodeling feature is reasonable. For example, suppose that the global analysis were continued with a fourth step of general, nonlinear static response:
|
||||
|
||||
```txt
|
||||
*RESTART, READ, STEP=3
|
||||
** Read state at end of initial preload
|
||||
** (could equally well use *RESTART, READ, STEP=1)
|
||||
*STEP
|
||||
** Add more preload
|
||||
*STATIC
|
||||
0.2, 1.0
|
||||
...
|
||||
*END STEP
|
||||
```
|
||||
|
||||
This fourth general analysis step starts with the state at the end of general analysis Step 1 because the frequency extraction and the modal dynamic steps are both linear perturbation steps. However, if we restart the submodel analysis in the same way, the solution may not be comparable with the global model solution:
|
||||
|
||||
```csv
|
||||
*RESTART, READ, STEP=2
|
||||
** Read state at end of step 2
|
||||
*STEP
|
||||
** Add more preload
|
||||
*STATIC
|
||||
0.2, 1.0
|
||||
*BOUNDARY, SUBMODEL, STEP=4
|
||||
...
|
||||
*END STEP
|
||||
```
|
||||
|
||||
The second step in the submodel is a general analysis step, to which the response may be nonlinear, thus changing the state of the model. A valid alternative would be to apply the Step 4 response to the submodel immediately after the first step:
|
||||
|
||||
```txt
|
||||
*RESTART, READ, STEP=1
|
||||
** Read state at end of preload step
|
||||
*STEP
|
||||
```
|
||||
|
||||
<!-- source-page: 783 -->
|
||||
|
||||
```csv
|
||||
** Add more preload
|
||||
*STATIC
|
||||
0.2, 1.0
|
||||
*BOUNDARY, SUBMODEL, STEP=4
|
||||
...
|
||||
*END STEP
|
||||
```
|
||||
|
||||
# Reinterpreting solution variables in the submodel analysis
|
||||
|
||||
During general analysis steps Abaqus works in terms of total solution variables such as the displacements, . In linear perturbation steps Abaqus works in terms of the displacement perturbation, $\Delta u ,$ , about a base state, $u \big \vert _ { 0 } .$ . When general analysis steps and linear perturbation steps are reinterpreted in the submodel analysis, the global analysis results are treated as defined in Table 10.2.2–1.
|
||||
|
||||
Table 10.2.2–1 Reinterpreting solution variables in the submodel analysis.
|
||||
|
||||
<table><tr><td>Global analysis step basis</td><td>Submodel step basis</td><td>Global increment specified in definition of submodel boundary condition</td><td>Driven variable basis</td></tr><tr><td>General</td><td>General</td><td>none</td><td> $u_s = u_g$ </td></tr><tr><td>Linear perturbation</td><td>General</td><td>none</td><td> $u_s = u_s|_0 + \Delta u_g$ </td></tr><tr><td>General</td><td>Static, linear perturbation</td><td>i</td><td> $\Delta u_s = u_g|_i - u_s|_0$ </td></tr><tr><td>Linear perturbation</td><td>Static, linear perturbation</td><td>i</td><td> $\Delta u_s = \Delta u_g|_i$ </td></tr></table>
|
||||
|
||||
In this table
|
||||
|
||||
<table><tr><td> $u_s$ </td><td>is the current value of a driven variable in the submodel at any time during a general, nonlinear, analysis step;</td></tr><tr><td> $\Delta u_s$ </td><td>is the value of the perturbation of a driven variable in the submodel during a linear perturbation step;</td></tr><tr><td> $u_g$ and $\Delta u_g$ </td><td>are the corresponding values of the same (geometrically interpolated) variable in the global model;</td></tr><tr><td> $u_g|_0$ </td><td>is the “base state” value of the variable during a linear perturbation step in the global analysis;</td></tr><tr><td> $u_s|_0$ </td><td>is the “base state” value of the variable during a linear perturbation step in the submodel analysis;</td></tr></table>
|
||||
|
||||
<!-- source-page: 784 -->
|
||||
|
||||
$$
|
||||
\begin{array}{l} u _ {g} | _ {i} \quad \text { is the value of } u _ {g} \text { at increment } i \text { of the global analysis step; and } \\ \Delta u _ {g} | _ {i} \quad \text { is the value of } \Delta u _ {g} \text { at increment } i \text { of the global analysis step. } \\ \end{array}
|
||||
$$
|
||||
|
||||
# Mixing general and linear perturbation steps in shell-to-solid submodeling
|
||||
|
||||
Additional assumptions must be made for the shell-to-solid case when a general procedure on the global model drives a linear perturbation procedure on the submodel and vice versa. The assumptions depend on the geometric formulation used (linear or nonlinear) and on the procedure combination. For details and governing equations for these cases, see “Submodeling analysis,” Section 2.15.1 of the Abaqus Theory Guide.
|
||||
|
||||
# Initial conditions
|
||||
|
||||
The definition of initial conditions should be consistent between the global model and the submodel.
|
||||
|
||||
# Boundary conditions
|
||||
|
||||
Boundary conditions (other than submodel boundary conditions) prescribed on the degrees of freedom that are driven will replace those prescribed using submodel boundary conditions. When this replacement occurs, Abaqus reports the change in the data file.
|
||||
|
||||
A node can be driven from the global model in some steps and have user-prescribed boundary conditions in other steps. In these cases all relevant boundary conditions must be respecified (see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1).
|
||||
|
||||
Any other boundary conditions that are applied in the submodel region should be imposed in the submodel analysis in the usual way. It is your responsibility to apply such prescribed boundary conditions to the submodel correctly so that they correspond to the loading of the global model.
|
||||
|
||||
Be careful with submodel boundary nodes that are also on planes of symmetry, where both forms of boundary conditions can be applied. It may be helpful in such cases to apply boundary conditions in a local coordinate system (see “Transformed coordinate systems,” Section 2.1.5). The local coordinate system should be applied only to the boundary conditions that are intended to override the submodel boundary conditions, since the submodel boundary conditions are always output in the global coordinate directions by the global model.
|
||||
|
||||
# Loads
|
||||
|
||||
Any loads that are applied in the submodel region must be imposed in the submodel analysis in the usual way. It is your responsibility to apply such loads to the submodel correctly so that they correspond to the loading of the global model. See “Applying loads: overview,” Section 34.4.1, for an overview of the loads available in Abaqus.
|
||||
|
||||
# Predefined fields
|
||||
|
||||
The following predefined fields can be specified in a submodeling analysis, as described in “Predefined fields,” Section 34.6.1:
|
||||
|
||||
<!-- source-page: 785 -->
|
||||
|
||||
• Nodal temperatures can be specified. Any difference between the applied and initial temperatures will cause thermal strain if a thermal expansion coefficient is given for the material (“Thermal expansion,” Section 26.1.2). The specified temperature also affects temperature-dependent material properties, if any.
|
||||
• The values of user-defined field variables can be specified. These values affect only field-variabledependent material properties, if any.
|
||||
|
||||
Abaqus interpolates solution variables onto the submodel driven nodes. It can also interpolate temperatures as field variables (see “Interpolating data between meshes” in “Predefined fields,” Section 34.6.1, for details). Other predefined fields will not be interpolated to the nodes of the submodel; they must be available from the input data for all nodes of the submodel where they are required.
|
||||
|
||||
Abaqus/Standard provides multiple approaches for cases where a submodel thermal-stress analysis must be performed using temperature solutions from a global heat transfer analysis.
|
||||
|
||||
• Run a heat transfer analysis of the global model, and write the nodal temperatures to the results or output database file. Run a sequentially coupled thermal-stress analysis of the global model. The temperatures obtained from the results or output database file of the global heat transfer analysis are field variables in this case. If the mesh used in the thermal-stress analysis is different from the mesh in the heat transfer analysis, specify that Abaqus/Standard should interpolate the temperature field from the heat transfer analysis mesh to the thermal-stress analysis mesh. Run a thermalstress analysis of the submodel using the results or output database file for the global thermal-stress analysis to read the driven variables (displacement field) and using the results or output database file from either the global heat transfer analysis or the global thermal-stress analysis to read the temperatures as field variables. In either case the temperature field will have to be interpolated to the current submodel nodes. If interpolation between dissimilar meshes is necessary, the global output database file must be used to read the temperatures. For details, see Figure 10.2.2–13 and Figure 10.2.2–14.
|
||||
|
||||
|
||||
|
||||
<details>
|
||||
<summary>flowchart</summary>
|
||||
|
||||
```mermaid
|
||||
graph TD
|
||||
A["Global model (mesh1)\nHeat transfer analysis"] --> B["Field variables\nGlobal.odb\nInterpolate from\nmesh1 to mesh 3"]
|
||||
A --> C["Field variables\nGlobal.odb\nInterpolate from\nmesh1 to mesh4"]
|
||||
B --> D["Global model (mesh3)\nStatic analysis\nRead temperatures from Global.odb"]
|
||||
C --> E["Submodel (mesh4)\nStatic analysis\nRead temperatures from Global.odb"]
|
||||
D --> F["Driven variables\nGlobal_u.fil or Global_u.odb"]
|
||||
E --> F
|
||||
```
|
||||
</details>
|
||||
|
||||
Figure 10.2.2–13 Sequentially coupled thermal-stress analysis for the global model with only a thermal-stress analysis for the submodel.
|
||||
|
||||
• Run a heat transfer analysis of the global model, and write the nodal temperatures to the results or output database file. Run a sequentially coupled thermal-stress analysis (the global thermal-stress
|
||||
|
||||
<!-- source-page: 786 -->
|
||||
|
||||
|
||||
|
||||
<details>
|
||||
<summary>flowchart</summary>
|
||||
|
||||
```mermaid
|
||||
graph TD
|
||||
A["Global model (mesh1)\nHeat transfer analysis"] --> B["Field variable\nGlobal_1.odb\nInterpolate from\nmesh1 to mesh2"]
|
||||
B --> C["Global model (mesh2)\nStatic analysis\nRead temperatures from Global_1.odb"]
|
||||
C --> D["Driven variable\nGlobal_2.fil or Global_2.odb"]
|
||||
C --> E["Field variable\nGlobal_2.odb\nInterpolate from\nmesh2 to mesh3"]
|
||||
D --> F["Submodel (mesh3)\nStatic analysis\nRead temperatures from Global_2.odb"]
|
||||
E --> F
|
||||
```
|
||||
</details>
|
||||
|
||||
Figure 10.2.2–14 Sequentially coupled thermal-stress analysis for the global model with only a thermal-stress analysis for the submodel.
|
||||
|
||||
analysis) using the same mesh (mesh1) as the global heat transfer analysis and the temperatures from the results or output database file for the global heat transfer analysis. Next, run a submodel heat transfer analysis using the mesh (mesh2) that is required for the final submodel thermal-stress analysis, and write the nodal temperatures to the results or output database file. Use the temperature solution from the global heat transfer analysis to drive the solution of the submodel heat transfer analysis. Finally, run the submodel thermal-stress analysis using the temperatures (as field variables) obtained from the results or output database file for the submodel heat transfer analysis and the displacements (as driven variables) obtained from the global thermal-stress analysis. See the detailed flow chart in Figure 10.2.2–15.
|
||||
|
||||
# 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:
|
||||
|
||||
<!-- source-page: 787 -->
|
||||
|
||||
|
||||
|
||||
<details>
|
||||
<summary>flowchart</summary>
|
||||
|
||||
```mermaid
|
||||
graph TD
|
||||
A["Global model (mesh1)\nHeat transfer analysis"] --> B["Field variables\nGlobal.fil or Global.odb"]
|
||||
B --> C["Global model (mesh1)\nStatic analysis\nRead temperatures from\nGlobal.fil or Global.odb"]
|
||||
C --> D["Driven variables\nGlobal.fil\nGlobal.odb"]
|
||||
D --> E["Driven variables\nGlobal_u.fil\nGlobal_u.odb"]
|
||||
E --> F["Submodel (mesh2)\nSubmodel\nHeat transfer analysis"]
|
||||
F --> G["Field variables\nSubmodel_heat.fil\nor\nSubmodel_heat.odb"]
|
||||
G --> H["Submodel (mesh2)\nStatic analysis\nRead temperatures from\nSubmodel_heat.fil or Submodel_heat.odb"]
|
||||
```
|
||||
</details>
|
||||
|
||||
Figure 10.2.2–15 Sequentially coupled thermal-stress analysis for both the global model and submodel.
|
||||
|
||||
• 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.
|
||||
|
||||
• When shell elements with five degrees of freedom per node (S4R5, S8R5, STRI65, etc.) are used in the global model, the rotations are not written to the results file or the output database; therefore, only the displacement degrees of freedom can be driven. This restriction suggests that submodeling should not be used with these elements or that the submodel should include a set of narrow elements around its driven edges so that the interpolated displacements at these nodes effectively transfer the rotation. Five degree of freedom shells cannot be used in shell-to-solid submodeling.
|
||||
|
||||
• 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, 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.
|
||||
|
||||
<!-- source-page: 788 -->
|
||||
|
||||
# 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.
|
||||
|
||||
# Input file template
|
||||
|
||||
Global analysis:
|
||||
```txt
|
||||
*HEADING
|
||||
...
|
||||
*STEP
|
||||
Step 1
|
||||
*STATIC (or *DYNAMIC, etc.)
|
||||
Data line to define step time and control incrementation
|
||||
...
|
||||
*NODE FILE
|
||||
List of solution variables to be used to drive the submodel
|
||||
*OUTPUT, FIELD
|
||||
*NODE OUTPUT
|
||||
List of solution variables to be used to drive the submodel
|
||||
*END STEP
|
||||
```
|
||||
|
||||
Submodel analysis:
|
||||
```txt
|
||||
*HEADING
|
||||
...
|
||||
*SUBMODEL, EXTERIOR TOLERANCE=tolerance
|
||||
List of all nodes to be driven
|
||||
**
|
||||
*STEP
|
||||
*STATIC (or any other allowable procedure)
|
||||
Data line to define step time (must be the same as the step time in the global analysis unless the TIMESCALE parameter is used on the *BOUNDARY option) and control incrementation
|
||||
...
|
||||
*BOUNDARY, SUBMODEL, STEP=1
|
||||
Data lines listing nodes and degrees of freedom to be driven in this step
|
||||
...
|
||||
*END STEP
|
||||
```
|
||||
|
||||
<!-- source-page: 789 -->
|
||||
|
||||
# 10.2.3 SURFACE-BASED SUBMODELING
|
||||
|
||||
# Products: Abaqus/Standard
|
||||
|
||||
# References
|
||||
|
||||
• “Submodeling: overview,” Section 10.2.1
|
||||
• \*SUBMODEL
|
||||
• \*DSLOAD
|
||||
• Chapter 38, “Submodeling,” of the Abaqus/CAE User’s Guide
|
||||
|
||||
# Overview
|
||||
|
||||
The surface-based submodeling technique:
|
||||
|
||||
• may not provide the same level of accuracy as node-based submodeling;
|
||||
• should be used only when the node-based technique cannot provide adequate results;
|
||||
• is limited to stress-based solid-to-solid submodeling for general static procedures (see “Static stress analysis,” Section 6.2.2) in Abaqus/Standard;
|
||||
• applies surface tractions to submodel surfaces based on a stress field interpolated from the global model; and
|
||||
• can be combined with node-based submodeling of displacements (see “Node-based submodeling,” Section 10.2.2).
|
||||
|
||||
# Performing a surface-based submodeling analysis
|
||||
|
||||
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 surfaces on the appropriate parts of the boundary of the submodel. Thus, the response at the boundary of the local region is defined by the solution for the global model. The driven surfaces and any loads applied to the local region determine the solution in the submodel.
|
||||
|
||||
Surface-based submodeling should be used only when the node-based technique cannot provide adequate results. For a comparison of the two submodeling techniques and recommendations for their application, refer to “Submodeling: overview,” Section 10.2.1.
|
||||
|
||||
# Saving the results from the global model
|
||||
|
||||
The results from the global analysis must be saved at all elements required for the interpolation of the driven variables to the boundary surface of the submodel. Only the output database (in ODB or SIM format) can be used for this purpose.
|
||||
|
||||
In each step of the global model whose solution will be used to drive the submodel, write the stress results to the output database (see “Output to the output database,” Section 4.1.3).
|
||||
|
||||
<!-- source-page: 790 -->
|
||||
|
||||
Input File Usage: Use both of the following options:
|
||||
|
||||
\*OUTPUT, FIELD
|
||||
|
||||
\*ELEMENT OUTPUT
|
||||
|
||||
Abaqus/CAE Usage: Step module: Output→Field Output Requests→Create
|
||||
|
||||
# Referring to the global model results from the submodel analysis
|
||||
|
||||
You must define the source of the global solution results and provide the name of the 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 ODB output database file or the SIM database file.
|
||||
|
||||
Input File Usage: abaqus job=submodel\_input\_file globalmodel= global\_output\_database or sim\_database\_file
|
||||
|
||||
Abaqus/CAE Usage: Any module: Model→Edit Attributes→submodel: Submodel:
|
||||
|
||||
Read data from job: global\_output\_database
|
||||
|
||||
Reading data from a SIM database file is not supported in Abaqus/CAE.
|
||||
|
||||
# Specifying the driven surfaces in the submodel
|
||||
|
||||
Specifying the driven element-based surfaces does not activate the driven surface loads: they must be activated by specifying the appropriate submodel distributed surface loads.
|
||||
|
||||
All surface facets of the submodel to be driven by stresses in any step must be specified as driven surfaces since the list of surfaces cannot be extended subsequent to its initial definition (even at restart). However, variables at the surfaces given do not have to be driven in all steps: the choice of which surfaces are driven in a particular step is made as part of a submodel distributed surface load definition, as discussed in “Defining the driven surface tractions in the submodel,” later in this section.
|
||||
|
||||
Input File Usage: \*SUBMODEL
|
||||
|
||||
list of element-based structural surfaces
|
||||
|
||||
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 surfaces specified on the data line of one option are separate and distinct from the other surfaces specified on the data lines of all the other options.
|
||||
|
||||
Abaqus/CAE Usage: Load module: Create Load: choose Other for the Category and Submodel
|
||||
|
||||
for the Types for Selected Step: Driving region: select region
|
||||
|
||||
# Defining geometric tolerances
|
||||
|
||||
A geometric tolerance is used to define how far driven element-based surface nodes 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, surface 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 surfaces lie to a greater extent outside
|
||||
Reference in New Issue
Block a user