In this blog post we will be discussing about the symmetric model generation feature that is incorporated in Abaqus. This feature is targeted towards reducing the solution time needed for an analysis. We will first present the supported features and limitations, followed by an exemplary analysis of a flanged connection wherein this feature can be used.
A 3d model can be created by:
A graphic detail of the supported features is shown in figure 1 below.
Figure 1: Supported geometry features (courtesy of Simulia).
Tip: Make sure you create sets and surfaces with meaningful names based on your modelling needs. You should also create full sets of the instances included in the original model. This will allow you to have display groups readily available for post processing. Remember that since the input file will be flat, you will not be able to select individual part instances from the viewport, rather than element or node sets.
The element type used in the original model, determines the element type in the new three-dimensional generated model. You can specify whether the new element should be either a general three-dimensional element or a cylindrical element. General and cylindrical elements can be used in the same model. There is also the option to discretize the generated model by applying biasing or by even customizing the number of elements per angular sector (for a revolved 3d generated model). The correspondence between axisymmetric and three dimensional element types can be found in the respectful section in the Abaqus documentation.
For our example, we will be using a 3d sector model (supported geometry feature no 2) representing a flange segment, comprising of two flange parts and an M48 bolt connecting them. First off, the pretensioning of the bolt will be performed. This type of loading is symmetric for the flange with respect its the symmetry axis. Next , this 3d sector model will be revolved around the symmetry axis in order to produce the generated model together with the solution fields (corresponding to the stresses-strains relating to pretensioning). The original model comprises of a 20 degree sector. The generated full flange 3d model will therefore comprise of 18 sectors and 18 bolts in total. As a subsequent analysis step, a moment around the Z-axis (unsymmetric loading) will be applied on the generated model.
A detail of the discretized original 3d sector model is shown in figure 2.
Figure 2: The discretized original 3d sector model.
A detail of the pretension stress results (view cut) are given in Figure 3.
Figure 3: Pretensioning step stress and contact pressure results.
As a first check, in order to check that the discretization of the generated model is adequate, and that the symmetric model generation feature works as expecte overall, we can run the following command via the cmd window. What is demonstrated next, focuses on purely geometry generation and not results transfer (yet).
We run the following command via the cmd--> “abaqus datacheck job=generated_model_full_3d.inp “
,where “generated_model_full_3d” corresponds to the input file of the generated model, followed by the input of the original model's name as shown in Figure 4.
Figure 4: Datacheck command window detail.
A detail and description of that input file is given in Figure 5.
Figure 5: Generated model input file detail for datacheck.
What is shown next in Figure 6, is the generated geometry upon running this input file via the cmd.
Figure 6: Generated geometry upon running the datacheck command on the generated model input file.
Up next , we will also transfer the results that were produced in the original sector model, and generate the solution field at the end of the sector model pretensioning analysis for the entire 3d geometry model. At the same input file, the subsequent step (that can correspond to an asymmetric load for example), together with its respectful loads, boundary conditions and output requests are included. The subsequent step will now exlusively concern the full 3d geometry. The detail of the generated model’s input file is given below, in Figure 7:
Figure 7: Generated model input file detail for results transfer and subsequent analysis.
A detail of the results of the full 3d model in terms of the change in contact pressure on the flange due to a bending moment acting on the full 3d geometry , is given below, in Figure 8.
A video of the deforrmation experience by the complete flange due to the bending action is given below.