Meshing has always been considered the most time-consuming task in the preprocessing phase of the Simulation, which is true as well. However, the complex geometry is considered as the only reason for long meshing hours. The task becomes more daunting for explicit models in which the hexahedral meshing is the priority to avoid element collapse and model stability during solve.
The meshing job can be complex for the simple geometry as well. One such scenario is a hybrid meshing in which multiple element topologies are involved. Common examples are honeycomb structures and civil structures with reinforcements. It can be very difficult to establish nodal connectivity manually between elements of different topologies in such situations.
This problem can be addressed by Abaqus CAE as it offers an automated hybrid meshing feature. This technique requires the user to define skins and stringers prior to meshing. These skins and stringers provide support for shell and beam elements generation that are fused at nodal locations to the underlying continuum solid elements. The result is a single hybrid mesh consisting of a three-dimensional matrix of continuum solid elements, two dimensional shells for skin and one-dimensional beams for reinforcements.
In this blog we will show the step-by-step process of such hybrid meshing in Abaqus CAE
We take the example of a 3D Block Matrix in green that has two skins at top and bottom in white and four stringers at vertical edges in red.
STEP1: Define the 3D Block and give it a name. Define the individual material properties for the matrix, the skin, and the stringer. This is the conventional material definition method.
STEP2: Go to the property module in CAE. Use the tools as shown to define a skin with two face supports and a stringer with four edges support. Once done, they should appear in the history tree.
STEP3: Define a solid section for 3D matrix, a shell section for the skin and a beam section for the stringers. Assign these sections to respective geometries using three section assignments. Use the thickness and beam cross section parameters as appropriate. For the given problem, I have used a shell of 2mm thickness and offset in appropriate direction and a circular beam of 1mm radius.
STEP4: This is important information that is easy to miss. Define the beam orientation vector for the stringers as shown below. This feature is in the property module. CAE will prompt user to define “n1” vector that should not coincide with the direction of beam. The “n1” is projected on a plane normal to the stringers and is taken as the direction of principal maximum moment of Area of the cross-section profile. In this problem the global Z is the stringer direction. Either global X or global Y can be taken as convenient definitions of n1 as the cross section is circular. However, in case of sections such as C channel, I channel or L channel, the n1 vector should be properly defined to correctly orient the channel in space.
STEP5: Render the geometry to make sure the skin and stringer are defined correctly. Go to the part display options from the “view” pull down menu and check the idealization options as shown.
If everything is correct, the model should appear as below:
STEP6: The model is ready for meshing now. It’s a bit of pre meshing work but now the user does not need to worry about meshing skin and stringer individually and nodal connectivity. Just mesh the 3D matrix as usual. The corresponding meshes for the skin and stringer are automatically defined and connected to the 3D block matrix.
STEP7: Run a query on elements to see all the element topologies. For this model, the element details are as follows. The model is now ready for further steps of simulation.
