Main Content

Modal Superposition Method for Structural Dynamics Problem

This example shows how to solve a structural dynamics problem by using modal analysis results. Solve for the transient response at the center of a 3-D beam under a harmonic load on one of its corners. Compare the direct integration results with the results obtained by modal superposition.

Modal Analysis

Create a modal analysis model for a 3-D problem.

modelM = createpde("structural","modal-solid");

Create the geometry and include it in the model. Plot the geometry and display the edge and vertex labels.

gm = multicuboid(0.05,0.003,0.003);
modelM.Geometry=gm;
pdegplot(modelM,"EdgeLabels","on","VertexLabels","on");
view([95 5])

Figure contains an axes object. The axes object contains 3 objects of type quiver, patch, line.

Generate a mesh.

msh = generateMesh(modelM);

Specify Young's modulus, Poisson's ratio, and the mass density of the material.

structuralProperties(modelM,"YoungsModulus",210E9, ...
                            "PoissonsRatio",0.3, ...
                            "MassDensity",7800);

Specify minimal constraints on one end of the beam to prevent rigid body modes. For example, specify that edge 4 and vertex 7 are fixed boundaries.

structuralBC(modelM,"Edge",4,"Constraint","fixed");
structuralBC(modelM,"Vertex",7,"Constraint","fixed");

Solve the problem for the frequency range from 0 to 500000. The recommended approach is to use a value that is slightly smaller than the expected lowest frequency. Thus, use -0.1 instead of 0.

Rm = solve(modelM,"FrequencyRange",[-0.1,500000]);

Transient Analysis

Create a transient analysis model for a 3-D problem.

modelD = createpde("structural","transient-solid");

Use the same geometry and mesh as for the modal analysis.

modelD.Geometry = gm;
modelD.Mesh = msh;

Specify the same values for Young's modulus, Poisson's ratio, and the mass density of the material.

structuralProperties(modelD,"YoungsModulus",210E9, ...
                            "PoissonsRatio",0.3, ...
                            "MassDensity",7800);

Specify the same minimal constraints on one end of the beam to prevent rigid body modes.

structuralBC(modelD,"Edge",4,"Constraint","fixed");
structuralBC(modelD,"Vertex",7,"Constraint","fixed");

Apply a sinusoidal force on the corner opposite the constrained edge and vertex.

structuralBoundaryLoad(modelD,"Vertex",5, ...
                              "Force",[0,0,10], ...
                              "Frequency",7600);

Specify the zero initial displacement and velocity.

structuralIC(modelD,"Velocity",[0;0;0],"Displacement",[0;0;0]);

Specify the relative and absolute tolerances for the solver.

modelD.SolverOptions.RelativeTolerance = 1E-5;
modelD.SolverOptions.AbsoluteTolerance = 1E-9;

Solve the model using the default direct integration method.

tlist = linspace(0,0.004,120);
Rd = solve(modelD,tlist);

Now, solve the model using the modal results.

tlist = linspace(0,0.004,120);
Rdm = solve(modelD,tlist,"ModalResults",Rm);

Interpolate the displacement at the center of the beam.

intrpUd = interpolateDisplacement(Rd,0,0,0.0015);
intrpUdm = interpolateDisplacement(Rdm,0,0,0.0015);

Compare the direct integration results with the results obtained by modal superposition.

plot(Rd.SolutionTimes,intrpUd.uz,"bo")
hold on
plot(Rdm.SolutionTimes,intrpUdm.uz,"rx")
grid on
legend("Direct integration", "Modal superposition")
xlabel("Time");
ylabel("Center of beam displacement")

Figure contains an axes object. The axes object contains 2 objects of type line. These objects represent Direct integration, Modal superposition.