Oct 16, 2023
Version 2
Simulating the modal analysis of hyperelastic membranes immersed in fluid using FE software ANSYS V.2
- 1Platform of Hydraulic Constructions (PL-LCH), Ecole Polytechnique Fédérale de Lausanne (EPFL)
Protocol Citation: samuel.vorlet Vorlet 2023. Simulating the modal analysis of hyperelastic membranes immersed in fluid using FE software ANSYS. protocols.io https://dx.doi.org/10.17504/protocols.io.bp2l6x7dklqe/v2Version created by samuel.vorlet Vorlet
License: This is an open access protocol distributed under the terms of the Creative Commons Attribution License, which permits unrestricted use, distribution, and reproduction in any medium, provided the original author and source are credited
Protocol status: Working
We use this protocol and it's working
Created: October 06, 2023
Last Modified: October 16, 2023
Protocol Integer ID: 88915
Keywords: Modal analysis, Hyperelastic, ANSYS, Fluid-structure interactions
Abstract
This protocol provides step-by-step guidelines to perform the modal analysis of pre-strained hyperelastic rectangular membrane accounting for fluid-structure interactions using Finite Element software ANSYS (Workbench). The nonlinear constitutive behavior of the material is modeled by the Mooney-Rivlin equation. The effect of water is considered by the added mass approach. The damping is included as Rayleigh damping.
Hyperelastic material definition using the Mooney-Rivlin formulation from uniaxial test data
Hyperelastic material definition using the Mooney-Rivlin formulation from uniaxial test data
Open Engineering Data.
Ad a new material and define the material name. Verify the units.
Define the hyperelastic material properties.
In the Hyperelastic Experimental Data, include the Uniaxial Test Data.
In the Uniaxial Test Data, define the Strain (mm^-1) and Stress (Pa) values from the uniaxial test data.
In the Hyperelastic toolbox, choose the Mooney-Rivlin material model with the appropriate number of parameters (double-click on it). The number of parameters for the Mooney-Rivlin depends on the shape of the stress-strain curve and the number of inflexion points.
In the Curve Fitting toolbox, choose the Mooney-Rivlin X parameters to add it to the material properties. Solve the curve fitting for the uniaxial test data (right-click on Curve Fitting -> Solve Curve Fit). Then, transfer the calculated values to the Mooney-Rivlin material constants (right-click on Curve Fitting -> Copy Calculated Values to Property). Verify that the material constants are correctly inserted. Verify the Incompressibility Parameter (D1 = 0 for incompressible materials).
Define the material density. In the Physical Properties toolbox, include the Density and define it.
When considering the added mass effect, the effective density should be defined. The added mass relies on the geometry and dimensions of the specimen and the density of the fluid . For a rectangular specimen:
where is a constant and depends on the ratio (sides of the specimen). The added density is obtained by dividing the added mass by the volume of the specimen:
Last, the effective density is defined as:
where is the structural density.
Static analysis to define the initial conditions for the modal analysis (accounting for nonlinearities)
Static analysis to define the initial conditions for the modal analysis (accounting for nonlinearities)
Drag the Static Structural analysis from the toolbox over the Engineering Data module. Open the static structural analysis by double-clicking on the Setup component.
Draw or import the Geometry.
Define the analysis setup by opening the Model (starting ANSYS Mechanical).
Assign the material to the body. Select the Geometry in the outline, then select the SYS\body. Under Details of SYS\body, assign the Material by selecting the previously defined material.
Define the mesh properties by selecting the Mesh in the outline. Verify the Physics Preference (Mechanical) and the Element Order (Quadratic). In the Sizing, define the appropriate characteristics. The mesh can be refined by adding elements to the mesh characteristics (right-click on the Mesh in the outline -> Insert -> Sizing/Refinement/Inflation/etc.).
Define the element type for the meshing by selecting the Geometry in the outline, select the SYS\body and insert an APDL commande snippet (right-click -> Insert -> Commands). Use the following APDL code to define the desired mesh element type (for instance SOLID187):
Define the analysis setup by selecting Static Structural in the outline.
Activate nonlinear analysis by turning ON the Large Deflection in the Solver Controls.
Insert gravity effects on the Analysis Settings in the outline (right-click -> Insert -> Standard Earth Gravity). Define the desired Z Component of the gravity (m/s^2).
Define the boundary conditions by selecting the Analysis Settings in the outline (right-click -> Insert -> Fixed Supprt/Displacement/etc.). Assign the boundary to the geometry part (Geometry Selection) and define the boundary type (Fixed Support for instance).
Define the external load (hydrostatic pressure) by selecting the Analysis Settings in the outline (right-click -> Insert -> Hydrostatic Pressure). Select the face where to apply the hydrostatic pressure (Scope -> Geometry), define the fluid density (Definition -> Fluid Density) and the magnitude of the hydrostatic pressure (Free Surface Location -> Z Coordinate).
Define the pre-strain by selecting the Geometry in the outline, select the SYS\body and insert an APDL command snippet using the INISTATE command (right-click -> Insert -> Commands). The following APDL code must be used:
cmsel,s,body,elem !Geometry selection (here body, to be adapted)
INISTATE,SET,DTYP,STRE !Set stress value, in Pa
INISTATE,DEFINE,,,,,500000,0,0,,, !Define the stress value (here, 0.5 MPa)
ALLSEL
Run the static analysis by selecting the Static Structural in the Outline (right-click -> Solve).
Visualize the results by selecting Solution in the outline (right-click -> Insert ->Deformation/Strain/Stress/etc.). After adding the results type, right-click on Solution in the Outline and select Evaluate All Results.
Modal analysis of a pre-strained hyperelastic material
Modal analysis of a pre-strained hyperelastic material
Drag the Modal analysis from the toolbox over the Solution of the Static Structural module. Open the modal analysis by double-clicking on the Setup component.
Define the number of modes to calculate by selecting the Analysis Settings in the Modal in the Outline. In Details of Analysis Settings, define the Max Modes to Find.
When considering the damping effect, the damping must be inserted by selecting Analysis Settings in the Outline and Solver Controls -> Damped -> Yes. Then, the damping parameters must be given under Damping Controls.
The damping is defined as Rayleigh damping (linear combination of mass and stiffness):
The coefficients are frequency-dependent and are given by:
where is the -th mode natural circular frequency in vacuum and is the corresponding damping ratio. The -th natural frequencies are determined using the FE numerical model in vacuum.
Run the modal analysis by selecting the Modal in the Outline (right-click -> Solve). The natural frequencies can be found by clicking on the Solution Information of the Solution.
Visualize the results (mode shapes) by selecting Solution in the outline (right-click -> Insert ->Total Deformation) and choose the mode number by selecting Total Deformation and Mode. After adding the results type, right-click on Solution in the Outline and select Evaluate All Results.