TransientStructuralResults
Transient structural solution and derived quantities
Description
A TransientStructuralResults object contains
the displacement, velocity, and acceleration in a form convenient for plotting and
postprocessing.
Displacement, velocity, and acceleration are reported for the nodes of the triangular
or tetrahedral mesh generated by generateMesh. The displacement, velocity, and acceleration values at the
nodes appear as FEStruct objects in the
Displacement, Velocity, and
Acceleration properties. The properties of these objects contain
the components of the displacement, velocity, and acceleration at the nodal
locations.
To evaluate the stress, strain, von Mises stress, principal stress, and principal
strain at the nodal locations, use evaluateStress, evaluateStrain, evaluateVonMisesStress, evaluatePrincipalStress, and evaluatePrincipalStrain, respectively.
To evaluate the reaction forces on a specified boundary, use evaluateReaction.
To interpolate the displacement, velocity, acceleration, stress, strain, and von Mises
stress to a custom grid, such as the one specified by meshgrid, use interpolateDisplacement, interpolateVelocity, interpolateAcceleration, interpolateStress, interpolateStrain, and interpolateVonMisesStress, respectively.
Creation
Solve a dynamic linear elasticity problem by using the solve function. This function returns a transient structural solution as
a TransientStructuralResults object.
Properties
Object Functions
evaluateStress | Evaluate stress for dynamic structural analysis problem |
evaluateStrain | Evaluate strain for dynamic structural analysis problem |
evaluateVonMisesStress | Evaluate von Mises stress for dynamic structural analysis problem |
evaluateReaction | Evaluate reaction forces on boundary |
evaluatePrincipalStress | Evaluate principal stress at nodal locations |
evaluatePrincipalStrain | Evaluate principal strain at nodal locations |
filterByIndex | Access transient results for specified time steps |
interpolateDisplacement | Interpolate displacement at arbitrary spatial locations |
interpolateVelocity | Interpolate velocity at arbitrary spatial locations for all time or frequency steps for dynamic structural problem |
interpolateAcceleration | Interpolate acceleration at arbitrary spatial locations for all time or frequency steps for dynamic structural problem |
interpolateStress | Interpolate stress at arbitrary spatial locations |
interpolateStrain | Interpolate strain at arbitrary spatial locations |
interpolateVonMisesStress | Interpolate von Mises stress at arbitrary spatial locations |
Examples
Solve for the transient response of a thin 3-D plate under a harmonic load at the center.
Create a geometry of a thin 3-D plate and plot it.
gm = multicuboid([5,0.05],[5,0.05],0.01);
pdegplot(gm,FaceLabels="on",FaceAlpha=0.5)
Zoom in to see the face labels on the small plate at the center.
figure
pdegplot(gm,FaceLabels="on",FaceAlpha=0.25)
axis([-0.2 0.2 -0.2 0.2 -0.1 0.1])
Create an femodel object for transient structural analysis and include the geometry.
model = femodel(AnalysisType="structuralTransient", ... Geometry=gm);
Specify Young's modulus, Poisson's ratio, and the mass density of the material.
model.MaterialProperties = ... materialProperties(YoungsModulus=210E9, ... PoissonsRatio=0.3, ... MassDensity=7800);
Specify that all faces on the periphery of the thin 3-D plate are fixed boundaries.
model.FaceBC(5:8) = faceBC(Constraint="fixed");Apply a sinusoidal pressure load on the small face at the center of the plate.
First, define a sinusoidal load function, sinusoidalLoad, to model a harmonic load. This function accepts the load magnitude (amplitude), the location and state structure arrays, frequency, and phase. Because the function depends on time, it must return a matrix of NaN of the correct size when state.time is NaN. Solvers check whether a problem is nonlinear or time-dependent by passing NaN state values and looking for returned NaN values.
function Tn = sinusoidalLoad(load,location,state,Frequency,Phase) if isnan(state.time) Tn = NaN*(location.nx); return end if isa(load,"function_handle") load = load(location,state); else load = load(:); end % Transient model excited with harmonic load Tn = load.*sin(Frequency.*state.time + Phase); end
Now, apply a sinusoidal pressure load on face 12 by using the sinusoidalLoad function.
Pressure = 5e7;
Frequency = 25;
Phase = 0;
pressurePulse = @(location,state) ...
sinusoidalLoad(Pressure,location,state,Frequency,Phase);
model.FaceLoad(12) = faceLoad(Pressure=pressurePulse);Generate a mesh with linear elements.
model = generateMesh(model,GeometricOrder="linear",Hmax=0.2);Specify zero initial displacement and velocity.
model.CellIC = cellIC(Displacement=[0;0;0],Velocity=[0;0;0]);
Solve the model.
tlist = linspace(0,1,300); R = solve(model,tlist);
The solver finds the values of the displacement, velocity, and acceleration at the nodal locations. To access these values, use R.Displacement, R.Velocity, and so on. The displacement, velocity, and acceleration values are returned as FEStruct objects with the properties representing their components. Note that properties of an FEStruct object are read-only.
R.Displacement
ans =
FEStruct with properties:
ux: [2217×300 double]
uy: [2217×300 double]
uz: [2217×300 double]
Magnitude: [2217×300 double]
R.Velocity
ans =
FEStruct with properties:
vx: [2217×300 double]
vy: [2217×300 double]
vz: [2217×300 double]
Magnitude: [2217×300 double]
R.Acceleration
ans =
FEStruct with properties:
ax: [2217×300 double]
ay: [2217×300 double]
az: [2217×300 double]
Magnitude: [2217×300 double]
Version History
Introduced in R2018a
See Also
Functions
solve|evaluateStress|evaluateStrain|evaluateVonMisesStress|evaluateReaction|evaluatePrincipalStress|evaluatePrincipalStrain|interpolateDisplacement|interpolateVelocity|interpolateAcceleration|interpolateStress|interpolateStrain|interpolateVonMisesStress
