Hydrodynamic elements allow for the simulation of the interaction of fluids with solids without considering the details of the flow. These elements are suited for well contained fluids since the motion of the fluid, such as sloshing, is not taken into account. Such interaction between fluid and solids is typically done using hydrostatic pressure loads; however, hydrodynamic elements provide for a much more accurate representation of the fluid-solid interaction because they account for the inertia of the moving fluid.
Hydrodynamic element follows the assumption that the shear stress is negligible and that strain energy is only dependents upon volumetric strain:
U = 0.5*K*ε v 2
where K and ε v are the bulk modulus and volumetric strain respectively. This gives a normal hydrostatic bulk response as P = K*ε v .
3D hydrodynamic elements can have several geometric forms: bricks (8 corner nodes, 6 quadrilateral sides), pyramids (5 corner nodes, 1 quadrilateral side, 4 triangular sides), and tetrahedra (4 corner nodes, 4 triangular sides). Mid-side nodes are needed to better describe large-scale motion of the fluid.
Determination of Surface Numbers for 3D Hydrodynamic Elements
When applying loads to a surface number of a hydrodynamic part, be aware that some models may not have all the lines on the face to be loaded on the same surface number. What happens in this situation? If the model originated from a CAD solid model, all faces coincident with the surface of the CAD model will receive the load regardless of the surface number of the lines. In hand-built models and on CAD parts that are altered so that the part is no longer associated with the CAD part, the surface number that is common in any three of the four lines that define a face (four-node region) or two of the three lines (three-node region) determines the surface number of that face.
Next, select the integration order that will be used for the 3D hydrodynamic elements in this part in the Integration Order drop-down box. For rectangular shaped elements, select the 2nd Order option. For moderately distorted elements, select the 3rd Order option. For extremely distorted elements, select the 4th Order option. The computation time for element stiffness formulation increases as the third power of the integration order. Consequently, the lowest integration order which produces acceptable results should be used to reduce processing time.
For the 3D hydrodynamic elements in this part to have the midside nodes activated, select the Included option in the Midside Nodes drop-down box. If this option is selected, the 3D hydrodynamic elements will have additional nodes defined at the midpoints of each edge. (For meshes of CAD solid models, the midside nodes follow the original curvature of the CAD surface, depending on the option selected before creating the mesh. For hand-built models and CAD model meshes that are altered, the midside node is located at the midpoint between the corner nodes.) This will change an 8-node 3D hydrodynamic element into a 20-node 3D hydrodynamic element. An element with midside nodes will result in more accurately calculated gradients. Elements with midside nodes increase processing time. If the mesh is sufficiently small, then midside nodes may not provide any significant increase in accuracy.