김경종
173 lines
7.3 KiB
Markdown
173 lines
7.3 KiB
Markdown
<!-- source-page: 1361 -->
|
||
|
||
# Elements
|
||
|
||
Any of the heat transfer elements in Abaqus/Standard can be used in the thermal analysis. In the stress analysis the corresponding continuum or structural elements must be chosen. For example, if heat transfer shell element type DS4 is defined by nodes 100, 101, 102, and 103 in the heat transfer analysis, three-dimensional shell element type S4R or S4R5 must be defined by these nodes in the stress analysis procedure. For continuum elements heat transfer results from a mesh using first-order elements can be transferred to a stress analysis with a mesh using second-order elements (see “Using second-order stress elements with first-order heat transfer elements (the midside node capability)” in “Predefined fields,” Section 34.6.1).
|
||
|
||
# Output
|
||
|
||
The nodal temperatures must be written to the heat transfer analysis results or output database file by requesting the output variable NT (see “Output to the data and results files,” Section 4.1.2). These temperatures will be read into the stress analysis procedure.
|
||
|
||
Appropriate output variables are described in the heat transfer and stress analysis sections. All of the output variables are outlined in “Abaqus/Standard output variable identifiers,” Section 4.2.1.
|
||
|
||
# Input file template
|
||
|
||
A typical sequentially coupled thermal-stress analysis consists of two Abaqus/Standard runs: a heat transfer analysis and a subsequent stress analysis.
|
||
|
||
The following template shows the input for the heat transfer analysis heat.inp:
|
||
|
||
```txt
|
||
*HEADING
|
||
...
|
||
*ELEMENT, TYPE=DC2D4
|
||
(Choose the heat transfer element type)
|
||
...
|
||
*STEP
|
||
*HEAT TRANSFER
|
||
...
|
||
Apply thermal loads and boundary conditions
|
||
...
|
||
** Write all nodal temperatures to the results or
|
||
** output database file, heat.fil/heat.odb
|
||
*NODE FILE, NSET=NALL
|
||
NT
|
||
*OUTPUT, FIELD
|
||
*NODE OUTPUT, NSET=NALL
|
||
NT
|
||
*END STEP
|
||
```
|
||
|
||
<!-- source-page: 1362 -->
|
||
|
||
The following template shows the input for the subsequent static structural analysis:
|
||
|
||
```txt
|
||
*HEADING
|
||
...
|
||
* ELEMENT, TYPE=CPE4R
|
||
(Choose the continuum element type compatible with the heat transfer element type used)
|
||
...
|
||
* STEP
|
||
* STATIC
|
||
...
|
||
Apply structural loads and boundary conditions
|
||
...
|
||
* TEMPERATURE, FILE=heat
|
||
Read in all nodal temperatures from the results or output database file, heat.fil/heat.odb
|
||
...
|
||
* END STEP
|
||
```
|
||
|
||
<!-- source-page: 1363 -->
|
||
|
||
# 16.1.3 PREDEFINED LOADS FOR SEQUENTIAL COUPLING
|
||
|
||
Product: Abaqus/Standard
|
||
|
||
# References
|
||
|
||
• “Mapping thermal and magnetic loads,” Section 3.2.27
|
||
• “Defining an analysis,” Section 6.1.2
|
||
• “Eddy current analysis,” Section 6.7.5
|
||
• “Concentrated loads,” Section 34.4.2
|
||
|
||
# Overview
|
||
|
||
The values of the following whole element output quantities, generated in an Abaqus/Standard timeharmonic eddy current analysis, can be read into subsequent Abaqus/Standard analyses as point loads for sequentially coupled multiphysics workflows:
|
||
|
||
• Rate of Joule heat dissipation
|
||
• Magnetic body force intensity
|
||
|
||
A sequentially coupled multiphysics analysis can be used to apply electromagnetically generated loads (from a time-harmonic eddy current analysis) in a heat transfer, coupled temperature-displacement, or stress/displacement analysis. In many cases coupling is important only from the time-harmonic eddy current analysis; the impact of loading on the structure’s mechanical or thermal response is not great enough to affect the validity of the original time-harmonic eddy current analysis.
|
||
|
||
# Saving Joule heat dissipation or magnetic body force intensity for use in subsequent analyses
|
||
|
||
You can request Joule heat dissipation output (EMJH) or magnetic body force intensity output (EMBF) in a time-harmonic eddy current analysis. Only values stored in the output database (.odb) file are available for use with sequential coupling.
|
||
|
||
# Converting results for subsequent use
|
||
|
||
The whole element quantities are converted to nodal load quantities using the abaqus emloads utility. The utility converts Joule heat dissipation output to concentrated heat flux and magnetic body force intensity output to point loads. This utility also enables conversion of results between dissimilar meshes. For more information, see “Mapping thermal and magnetic loads,” Section 3.2.27.
|
||
|
||
# Conversion limitations
|
||
|
||
When converting results values between dissimilar meshes, global conservation of the net flux is ensured provided that the model domain in the heat transfer, coupled temperature-displacement, or stress/displacement analysis matches the model domain in the time-harmonic eddy current analysis.
|
||
|
||
<!-- source-page: 1364 -->
|
||
|
||
The conservative mapping algorithm used in the abaqus emloads utility also provides a locally smooth distribution of point flux values (either body force or concentrated heat flux) in cases where the mesh in the time-harmonic eddy current analysis is finer than the “target” representative mesh. In situations where this is not the case and the “target” representative mesh is finer or of similar size to the mesh in the time-harmonic eddy current analysis, you may observe nodal locations with zero converted flux values. In these cases you will still observe global conservation of the flux, but your solution may be adversely affected locally. You can correct for these situations by always performing the time-harmonic eddy current analysis with a finer mesh.
|
||
|
||
# Transferring nodal loads from the output database to concentrated loads
|
||
|
||
To define loads in a heat transfer, coupled temperature-displacement, or stress/displacement analysis, you can read nodal concentrated heat fluxes and point loads from the output database (.odb) file created by the abaqus emloads utility.
|
||
|
||
# Input file template
|
||
|
||
In this example heat flux values are stored in the output database from a time-harmonic eddy current analysis. These values, after conversion to point heat fluxes, are read into a subsequent analysis as a concentrated flux.
|
||
|
||
The following template shows the input for the time-harmonic eddy current analysis electromagnetic.inp:
|
||
|
||
```txt
|
||
*HEADING
|
||
...
|
||
*ELEMENT, TYPE=EMC3D8
|
||
(Choose the electromagnetic element type)
|
||
...
|
||
*STEP
|
||
*ELECTROMAGNETIC, LOW FREQUENCY, TIME HARMONIC
|
||
...
|
||
Apply loads and boundary conditions
|
||
...
|
||
** Write element Joule heat dissipation results to the output
|
||
** database file, electromagnetic.odb
|
||
*OUTPUT, FIELD
|
||
*ELEMENT OUTPUT, ELSET=CONDUCTOR
|
||
EMJH
|
||
*END STEP
|
||
```
|
||
|
||
The following template shows the input for the heat transfer analysis, heattransfer.inp, which refers to an output database, pointflux.odb, created using the abaqus emloads utility, and which has mapped quantities from the results of the time-harmonic eddy current analysis, stored in electromagnetic.odb:
|
||
|
||
<!-- source-page: 1365 -->
|
||
|
||
\*HEADING
|
||
|
||
\*ELEMENT, TYPE=DC3D8
|
||
|
||
(Choose the heat transfer continuum element type)
|
||
|
||
\*STEP
|
||
|
||
\*HEAT TRANSFER, STEADY STATE
|
||
|
||
Apply heat transfer loads and boundary conditions
|
||
|
||
\*CFLUX, FILE=pointflux.odb
|
||
|
||
Read in all nodal heat flux values from the output database and apply as concentrated nodal fluxes
|
||
|
||
\*END STEP
|
||
|
||
<!-- source-page: 1366 -->
|
||
|
||
<!-- source-page: 1367 -->
|
||
|
||
# 17. Co-simulation
|
||
|
||
Co-simulation 17.1
|
||
|
||
Preparing an Abaqus analysis for co-simulation 17.2
|
||
|
||
Co-simulation between Abaqus solvers 17.3
|
||
|
||
Co-simulation using Abaqus and discrete models 17.4
|
||
|
||
<!-- source-page: 1368 -->
|
||
|
||
<!-- source-page: 1369 -->
|
||
|
||
# 17.1 Co-simulation
|
||
|
||
• “Co-simulation: overview,” Section 17.1.1
|
||
|
||
<!-- source-page: 1370 -->
|