The most recent release of Autodesk’s advanced finite element analysis software, Inventor Nastran 2020, included some useful new features and upgrades. This includes automatic mesh convergence tools, Vault integration, corrected shell elements, and a new Hydrostatic load type.
This new load type allows the user to apply a fluid pressure that varies with the depth of fluid in a specific direction. Previous versions of Nastran In-CAD (2019 and earlier) required the user to create a variable pressure load using a table of coordinates and scalar multipliers. This approach also required the user to calculate the pressure at the bottom of the surface using the formula:
P = ρ*g*d
where the ρ (rho) is the fluid density, g is acceleration due to gravity, and d is the fluid depth. See the image below for more detail. Just like the standard Pressure load – the pressure will always act normal to the element face. NOTE: In Nonlinear Static studies, the pressure will continue to act normal to the surface even as it deforms.
Hydrostatic pressure loads can only be applied to the faces of shells and solids. With larger models and assemblies, it’s usually best to utilize shell elements to reduce the overall element count and prevent unusual stress concentrations. For the tank shown below, the walls are 1/4“ stainless steel. Due to the large size of the tank (10 ft. tall) a surface model was created so that shell elements can be easily applied. After applying a fine mesh the total element count is still only 10,000.
The process of applying a Hydrostatic Load is simple:
1. Create a new Load and use the drop-down menu to specify the type as “Hydrostatic Load.” There are no Sub Type selections for this load type.
2. Use the Fluid Density field to enter the weight density of the fluid causing the pressure. The default value will be 0.036 lbf/in^3 – the density of water.
3. Click In the “Point on Fluid Surface” box to activate the selection. Choose a work point, vertex, or use XYZ coordinates to define the top of the fluid. Only elements below this point will receive a hydrostatic pressure.
This work point can be created in the 3D model using Inventor’s work features on the 3D modeling tab. In this example – a work point was created 6 inches below the top of the tank to represent the maximum fluid volume height.
4. Define the fluid depth direction, either by selecting an entity in the model (work point or vertex), or by using the XYZ fields to define a vector. Typically it’s easiest to use the XYZ vector fields. In this example – the fluid depth direction is in the Z- direction. So the vector is entered as X=0, Y=0, Z= -1.
5. Use the arrow next to Fluid Depth Direction to change the normal direction that the pressure will be acting on the surface. The green arrows should be facing outwards in this example because the fluid is inside the tank. The arrows should also increase in size from the top to the bottom.
6. Constrain the model as required and run the analysis. In this example, the maximum displacement was 0.01” and the maximum Von Mises stress was 4198 psi.