ProductsAbaqus/StandardAbaqus/Explicit Elements testedSC8RT
Features testedThe submodeling capability is applied to two-dimensional, three-dimensional, and axisymmetric continuum coupled temperature-displacement elements. General steps invoking the steady-state coupled temperature-displacement and the dynamic temperature-displacement procedures are used in Abaqus/Standard and Abaqus/Explicit, respectively, for both the global and submodel analyses. Problem descriptionModel:All global models have dimensions 7.0 × 7.0 in the x–y or r–z plane. Each submodel has dimensions 5.0 × 5.0 in the x–y or r–z plane and occupies the lower right-hand corner of the corresponding global model. In all but the axisymmetric models, the out-of-plane dimension is 1.0. In axisymmetric models the structure analyzed is a hollow cylinder with an outer radius of 8.0. Material:In Abaqus/Standard:
In Abaqus/Explicit:
Loading:In all Abaqus/Standard models a distributed flux of magnitude 0.3 is applied to the right face; in Abaqus/Explicit the flux magnitude is 0.5× 104. Boundary and initial conditionsIn the global model fixed boundary conditions =0 and =0 are prescribed on the left and bottom faces, respectively. In three-dimensional models the additional constraints =0 are applied to the nodes on the front and back faces. The initial temperature is zero everywhere, and fixed temperature boundary conditions are applied on the left face. In the submodel =0 is prescribed everywhere on the bottom face, while degrees of freedom 1, 2, and 11 for the nodes on the top and left faces are being driven by the global solution. The mass scaling technique is used in the Abaqus/Explicit models to speed-up the analysis. Results and discussionIn the global analyses the temperature field predicted by Abaqus varies linearly in the x-direction in nonaxisymmetric models and logarithmically in the r-direction in axisymmetric models. The predicted displacement field is nonuniform in all models. The Abaqus/Standard results depicted for the temperature and x- or r-displacement contour plots are shown below. For comparison purposes the temperature and displacement solutions predicted by the submodels are also presented in the same contour plots, and excellent agreement between the global and submodel results is obtained. Hence, the amplitudes of all driven variables in the submodel analysis are identified correctly in the global analysis file output and applied at the driven nodes in the submodel analysis. Global and submodel analyses results for 4-node plane stress elements in Abaqus/Standard are shown in Figure 1 and Figure 2. Global and submodel Abaqus/Standard analyses results for 8-node plane strain elements are shown in Figure 3 and Figure 4. Global and submodel Abaqus/Standard analyses results for 8-node axisymmetric elements are shown in Figure 5 and Figure 6. Global and submodel Abaqus/Standard analyses results for 20-node brick elements (front face) are shown in Figure 7 and Figure 8. In Abaqus/Explicit the driven temperatures and displacements in the submodel are correctly interpolated from the global analysis file output. Each of the two-dimensional, three-dimensional, or axisymmetric submodels can be driven from any global model that has the same dimensionality. The results between the global model and submodel agree extremely well. Input filesAbaqus/Standard input filesThe following input files test the steady-state fully coupled thermal-stress procedure:
Abaqus/Explicit input files
Figures        | |||||||||||||||||||||||||||||||