solve

Solve structural analysis, heat transfer, or electromagnetic analysis problem

Domain-specific structural, heat transfer, and electromagnetic workflows are not recommended. New features might not be compatible with these workflows. For help migrating your existing code to the unified finite element workflow, see Migration from Domain-Specific to Unified Workflow.

Syntax

results = solve(fem)

results = solve(fem,tlist)

results = solve(fem,flist)

results = solve(fem,FrequencyRange=[omega1,omega2])

results = solve(fem,DecayRange=[lambda1,lambda2])

results = solve(fem,Snapshots=Tmatrix)

results = solve(fem,tlist,ModalResults=thermalModalR)

results = solve(fem,tlist,ModalResults=structuralModalR)

results = solve(fem,flist,ModalResults=structuralModalR)

results = solve(fem,tlist,ModalResults=structuralModalR,DampingZeta=z)

results = solve(fem,flist,ModalResults=structuralModalR,DampingZeta=z)

results = solve(fem,omega)

structuralStaticResults = solve(structuralStatic)

structuralTransientResults = solve(structuralTransient,tlist)

structuralFrequencyResponseResults = solve(structuralFrequencyResponse,flist)

structuralModalResults = solve(structuralModal,"FrequencyRange",[omega1,omega2])

structuralTransientResults = solve(structuralTransient,tlist,ModalResults=structuralModalR)

structuralFrequencyResponseResults = solve(structuralFrequencyResponse,flist,ModalResults=structuralModalR)

thermalSteadyStateResults = solve(thermalSteadyState)

thermalTransientResults = solve(thermalTransient,tlist)

thermalModalResults = solve(thermalModal,DecayRange=[lambda1,lambda2])

thermalModalResults = solve(thermalModal,Snapshots=Tmatrix)

thermalTransientResults = solve(thermalTransient,tlist,ModalResults=thermalModalR)

emagStaticResults = solve(emagmodel)

emagHarmonicResults = solve(emagmodel,Frequency=omega)

Description

results = solve(fem) solves the structural, thermal, or electromagnetic problem represented by the finite element analysis model fem.

results = solve(fem,tlist) returns the solution at the times specified in tlist.

results = solve(fem,flist) returns the solution at the frequencies specified in flist.

results = solve(fem,FrequencyRange=[omega1,omega2]) solves the structural modal analysis problem represented by the finite element analysis model fem for all modes in the frequency range [omega1,omega2]. Define omega1 as slightly lower than the lowest expected frequency and omega2 as slightly higher than the highest expected frequency. For example, if the lowest expected frequency is zero, then use a small negative value for omega1.

results = solve(fem,DecayRange=[lambda1,lambda2]) performs an eigen decomposition of a linear thermal problem represented by the finite element analysis model fem for all modes in the decay range [lambda1,lambda2]. The resulting modes enable you to:

• Use the modal superposition method to speed up a transient thermal analysis.

• Extract the reduced modal system to use, for example, in Simulink^®.

results = solve(fem,Snapshots=Tmatrix) obtains the modal basis of a linear or nonlinear thermal problem represented by the finite element analysis model fem using proper orthogonal decomposition (POD). You can use the resulting modes to speed up a transient thermal analysis or, if your thermal model is linear, to extract the reduced modal system.

results = solve(fem,tlist,ModalResults=thermalModalR), results = solve(fem,tlist,ModalResults=structuralModalR), and results = solve(fem,flist,ModalResults=structuralModalR) solve a transient thermal or structural problem or a frequency response structural problem, respectively, by using the modal superposition method to speed up computations. First, perform modal analysis to compute natural frequencies and mode shapes in a particular frequency or decay range. Then, use this syntax to invoke the modal superposition method. The accuracy of the results depends on the modes in the modal analysis results.

results = solve(fem,tlist,ModalResults=structuralModalR,DampingZeta=z) and results = solve(fem,flist,ModalResults=structuralModalR,DampingZeta=z) solve a transient or frequency response structural problem with modal damping using the results of modal analysis. Here, z is the modal damping ratio.

results = solve(fem,omega) solves a harmonic electromagnetic problem represented in fem at the frequencies specified in omega.

structuralStaticResults = solve(structuralStatic) returns the solution to the static structural analysis model represented in structuralStatic.

structuralTransientResults = solve(structuralTransient,tlist) returns the solution to the transient structural dynamics model represented in structuralTransient at the times specified in tlist.

structuralFrequencyResponseResults = solve(structuralFrequencyResponse,flist) returns the solution to the frequency response model represented in structuralFrequencyResponse at the frequencies specified in flist.

structuralModalResults = solve(structuralModal,"FrequencyRange",[omega1,omega2]) returns the solution to the modal analysis model for all modes in the frequency range [omega1,omega2]. Define omega1 as slightly lower than the lowest expected frequency and omega2 as slightly higher than the highest expected frequency. For example, if the lowest expected frequency is zero, then use a small negative value for omega1.

structuralTransientResults = solve(structuralTransient,tlist,ModalResults=structuralModalR) and structuralFrequencyResponseResults = solve(structuralFrequencyResponse,flist,ModalResults=structuralModalR) solves a transient and a frequency response structural model, respectively, by using the modal superposition method to speed up computations. First, perform modal analysis to compute natural frequencies and mode shapes in a particular frequency range. Then, use this syntax to invoke the modal superposition method. The accuracy of the results depends on the modes in the modal analysis results.

thermalSteadyStateResults = solve(thermalSteadyState) returns the solution to the steady-state thermal model represented in thermalSteadyState.

thermalTransientResults = solve(thermalTransient,tlist) returns the solution to the transient thermal model represented in thermalTransient at the times specified in tlist.

thermalModalResults = solve(thermalModal,DecayRange=[lambda1,lambda2]) performs an eigen decomposition of a linear thermal model thermalModal for all modes in the decay range [lambda1,lambda2]. The resulting modes enable you to:

• Use the modal superposition method to speed up a transient thermal analysis.

• Extract the reduced modal system to use, for example, in Simulink.

thermalModalResults = solve(thermalModal,Snapshots=Tmatrix) obtains the modal basis of a linear or nonlinear thermal model using proper orthogonal decomposition (POD). You can use the resulting modes to speed up a transient thermal analysis or, if your thermal model is linear, to extract the reduced modal system.

thermalTransientResults = solve(thermalTransient,tlist,ModalResults=thermalModalR) solves a transient thermal model by using the modal superposition method to speed up computations. First, perform modal decomposition to compute mode shapes for a particular decay range. Then, use this syntax to invoke the modal superposition method. The accuracy of the results depends on the modes in the modal analysis results.

emagStaticResults = solve(emagmodel) returns the solution to the electrostatic, magnetostatic, or DC conduction model represented in emagmodel.

emagHarmonicResults = solve(emagmodel,Frequency=omega) returns the solution to the harmonic electromagnetic analysis model represented in emagmodel at the frequencies specified in omega.

Examples

Solve Static Structural Problem

Solve a static structural problem representing a bimetallic cable under tension.

Create and plot a bimetallic cable geometry.

gm = multicylinder([0.01 0.015],0.05);
pdegplot(gm,FaceLabels="on", ...
            CellLabels="on", ...
            FaceAlpha=0.5)

Create an femodel object for static structural analysis and include the geometry.

model = femodel(AnalysisType="structuralStatic", ...
                Geometry=gm);

Specify Young's modulus and Poisson's ratio for each metal.

model.MaterialProperties(1) = ...
    materialProperties(YoungsModulus=110E9, ...
                       PoissonsRatio=0.28);
model.MaterialProperties(2) = ...
    materialProperties(YoungsModulus=210E9, ...
                       PoissonsRatio=0.3);

Specify that faces 1 and 4 are fixed boundaries.

model.FaceBC([1,4]) = faceBC(Constraint="fixed");

Specify the surface traction for faces 2 and 5.

model.FaceLoad([2,5]) = faceLoad(SurfaceTraction=[0;0;100]);

Generate a mesh and solve the problem.

model = generateMesh(model);
R = solve(model)

R = 
  StaticStructuralResults with properties:

      Displacement: [1x1 FEStruct]
            Strain: [1x1 FEStruct]
            Stress: [1x1 FEStruct]
    VonMisesStress: [23098x1 double]
              Mesh: [1x1 FEMesh]

The solver finds the values of the displacement, stress, strain, and von Mises stress at the nodal locations. To access these values, use R.Displacement, R.Stress, and so on. The displacement, stress, and strain values at the nodal locations 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: [23098x1 double]
           uy: [23098x1 double]
           uz: [23098x1 double]
    Magnitude: [23098x1 double]

R.Stress

ans = 
  FEStruct with properties:

    sxx: [23098x1 double]
    syy: [23098x1 double]
    szz: [23098x1 double]
    syz: [23098x1 double]
    sxz: [23098x1 double]
    sxy: [23098x1 double]

R.Strain

ans = 
  FEStruct with properties:

    exx: [23098x1 double]
    eyy: [23098x1 double]
    ezz: [23098x1 double]
    eyz: [23098x1 double]
    exz: [23098x1 double]
    exy: [23098x1 double]

Plot the deformed shape with the z-component of normal stress.

pdeplot3D(R.Mesh, ...
          ColorMapData=R.Stress.szz, ...
          Deformation=R.Displacement)

Solve Transient Structural Problem

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: [2217x300 double]
           uy: [2217x300 double]
           uz: [2217x300 double]
    Magnitude: [2217x300 double]

R.Velocity

ans = 
  FEStruct with properties:

           vx: [2217x300 double]
           vy: [2217x300 double]
           vz: [2217x300 double]
    Magnitude: [2217x300 double]

R.Acceleration

ans = 
  FEStruct with properties:

           ax: [2217x300 double]
           ay: [2217x300 double]
           az: [2217x300 double]
    Magnitude: [2217x300 double]

Frequency Response Analysis

Perform frequency response analysis of a tuning fork.

Create an femodel object for frequency response analysis and include the geometry of a tuning fork in the model.

model = femodel(AnalysisType="structuralFrequency", ...
                Geometry="TuningFork.stl");

Specify Young's modulus, Poisson's ratio, and the mass density to model linear elastic material behavior. Specify all physical properties in consistent units.

model.MaterialProperties = ...
    materialProperties(YoungsModulus=210E9, ...
                       PoissonsRatio=0.3, ...
                       MassDensity=8000);

Identify faces for applying boundary constraints and loads by plotting the geometry with the face labels.

figure("units","normalized","outerposition",[0 0 1 1])
pdegplot(model,FaceLabels="on")
view(-50,15)
title("Geometry with Face Labels")

Impose sufficient boundary constraints to prevent rigid body motion under applied loading. Typically, you hold a tuning fork by hand or mount it on a table. To create a simple approximation of this boundary condition, fix a region near the intersection of tines and the handle (faces 21 and 22).

model.FaceBC([21,22]) = faceBC(Constraint="fixed");

Specify the pressure loading on a tine (face 11) as a short rectangular pressure pulse.

model.FaceLoad(11) = faceLoad(Pressure=1);

Generate a mesh. Specify the Hface name-value argument to generate a finer mesh for small faces.

model = generateMesh(model,Hmax=0.005,Hface={[3 4 9 10],0.0003});

In the frequency domain, this pressure pulse is a unit load uniformly distributed across all frequencies.

flist = linspace(0,4000,150);
R = solve(model,2*pi*flist);

Plot the vibration frequency of the tine tip, which is face 12. Find nodes on the tip face and plot the y-component of the displacement over the frequency, using one of these nodes.

excitedTineTipNodes = findNodes(model.Mesh,"region",Face=12);
tipDisp = R.Displacement.uy(excitedTineTipNodes(1),:);

figure 
plot(flist,abs(tipDisp)) 
xlabel("Frequency");
ylabel("|Y-Displacement|");

Solve Modal Structural Analysis Problem

Find the fundamental (lowest) mode of a 2-D cantilevered beam, assuming prevalence of the plane-stress condition.

Specify geometric and structural properties of the beam, along with a unit plane-stress thickness.

length = 5;
height = 0.1;
E = 3E7;
nu = 0.3;
rho = 0.3/386;

Create a geometry.

gdm = [3;4;0;length;length;0;0;0;height;height];
g = decsg(gdm,'S1',('S1')');

Create an femodel object for modal structural analysis and include the geometry.

model = femodel(Analysistype="structuralModal", ...
                Geometry=g);

Define a maximum element size (five elements through the beam thickness).

hmax = height/5;

Generate a mesh.

model=generateMesh(model,Hmax=hmax);

Specify the structural properties and boundary constraints.

model.MaterialProperties = ...
    materialProperties(YoungsModulus=E, ...
                       MassDensity=rho, ... 
                       PoissonsRatio=nu);
model.EdgeBC(4) = edgeBC(Constraint="fixed");

Compute the analytical fundamental frequency (Hz) using the beam theory.

I = height^3/12;
analyticalOmega1 = 3.516*sqrt(E*I/(length^4*(rho*height)))/(2*pi)

analyticalOmega1 = 
126.9498

Specify a frequency range that includes an analytically computed frequency and solve the model.

R = solve(model,FrequencyRange=[0,1e6])

R = 
  ModalStructuralResults with properties:

    NaturalFrequencies: [32x1 double]
            ModeShapes: [1x1 FEStruct]
                  Mesh: [1x1 FEMesh]

The solver finds natural frequencies and modal displacement values at nodal locations. To access these values, use R.NaturalFrequencies and R.ModeShapes.

R.NaturalFrequencies/(2*pi)

ans = 32×1
105 ×

    0.0013
    0.0079
    0.0222
    0.0433
    0.0711
    0.0983
    0.1055
    0.1462
    0.1930
    0.2455
      ⋮

R.ModeShapes

ans = 
  FEStruct with properties:

           ux: [6511x32 double]
           uy: [6511x32 double]
    Magnitude: [6511x32 double]

Plot the y-component of the solution for the fundamental frequency.

pdeplot(R.Mesh,XYData=R.ModeShapes.uy(:,1))
title(['First Mode with Frequency ', ...
        num2str(R.NaturalFrequencies(1)/(2*pi)),' Hz'])
axis equal

Solve Transient Structural Problem Using Modal Superposition Method

Solve for the transient response at the center of a 3-D beam under a harmonic load on one of its corners.

Modal Analysis

Create a beam geometry.

gm = multicuboid(0.05,0.003,0.003);

Plot the geometry with the edge and vertex labels.

pdegplot(gm,EdgeLabels="on",VertexLabels="on");
view([95 5])

Create an femodel object for modal structural analysis and include the geometry.

model = femodel(AnalysisType="structuralModal", ...
                Geometry=gm);

Generate a mesh.

model = generateMesh(model);

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 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.

model.EdgeBC(4) = edgeBC(Constraint="fixed");
model.VertexBC(7) = vertexBC(Constraint="fixed");

Solve the problem for the frequency range from 0 to 500,000. The recommended approach is to use a value that is slightly lower than the expected lowest frequency. Thus, use -0.1 instead of 0.

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

Transient Analysis

Switch the analysis type of the model to structural transient.

model.AnalysisType = "structuralTransient";

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

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)
    normal = [location.nx location.ny];
    if isfield(location,"nz")
        normal = [normal location.nz];
    end
    Tn = NaN*normal;
    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 force on vertex 5 by using the sinusoidalLoad function.

Force = [0,0,10];
Frequency = 7600;
Phase = 0;
forcePulse = @(location,state) ...
         sinusoidalLoad(Force,location,state,Frequency,Phase);
model.VertexLoad(5) = vertexLoad(Force=forcePulse);

Specify zero initial displacement and velocity.

model.CellIC = cellIC(Velocity=[0;0;0], ...
                      Displacement=[0;0;0]);

Specify the relative and absolute tolerances for the solver.

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

Solve the model using the modal results.

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

Interpolate and plot the displacement at the center of the beam.

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

plot(Rdm.SolutionTimes,intrpUdm.uz)
grid on
xlabel("Time");
ylabel("Center of beam displacement")

Expansion of Cantilever Beam Under Thermal Load

Find the deflection of a 3-D cantilever beam under a nonuniform thermal load. Specify the thermal load for the structural problem using the solution from a transient thermal analysis on the same geometry and mesh.

Transient Thermal Model Analysis

Create and plot the geometry.

gm = multicuboid(0.5,0.1,0.05);
pdegplot(gm,FaceLabels="on",FaceAlpha=0.3)

Create an femodel object for transient thermal analysis and include the geometry.

model = femodel(AnalysisType="thermalTransient", ...
                Geometry = gm);

Generate a mesh.

model = generateMesh(model);

Specify the thermal properties of the material.

model.MaterialProperties = ...
    materialProperties(ThermalConductivity=5e-3, ...
                       MassDensity=2.7*10^(-6), ...
                       SpecificHeat=10);

Specify the constant temperatures applied to the left and right ends of the beam.

model.FaceBC(3) = faceBC(Temperature=100);
model.FaceBC(5) = faceBC(Temperature=0);

Specify the heat source over the entire geometry.

model.CellLoad = cellLoad(Heat=10);

Set the initial temperature.

model.CellIC = cellIC(Temperature=0);

Solve the model.

tlist = 0:1e-4:2e-4;
thermalresults = solve(model,tlist);

Plot the temperature distribution for each time step.

for n = 1:numel(thermalresults.SolutionTimes)
    figure
    pdeplot3D(thermalresults.Mesh, ...
              ColorMapData=thermalresults.Temperature(:,n))
    title(["Temperature at Time = " ...
                num2str(tlist(n))])
end

Structural Analysis with Thermal Load

Switch the analysis type of the model to structural static.

model.AnalysisType = "structuralStatic";

Specify Young's modulus, Poisson's ratio, and the coefficient of thermal expansion.

model.MaterialProperties = ...
    materialProperties(YoungsModulus=1e10, ...
                       PoissonsRatio=0.3, ...
                       CTE=11.7e-6);

Apply a fixed boundary condition on face 5.

model.FaceBC(5) = faceBC(Constraint="fixed");

Apply a thermal load using the transient thermal results. By default, the toolbox uses the solution for the last time step.

model.CellLoad = cellLoad(Temperature=thermalresults);

Specify the reference temperature.

model.ReferenceTemperature = 10;

Solve the structural problem.

thermalstressresults = solve(model);

Plot the deformed shape of the beam corresponding to the last step of the transient thermal solution.

pdeplot3D(thermalstressresults.Mesh, ...
            "ColorMapData", ...
             thermalstressresults.Displacement.Magnitude, ...
            "Deformation", ...
             thermalstressresults.Displacement)
title(["Thermal Expansion at Solution Time = " ...
                         num2str(tlist(end))])

Now specify the thermal loads as the thermal results for all time steps. Access the results for each step by using the filterByIndex function. For each thermal load, solve the structural problem and plot the corresponding deformed shape of the beam.

for n = 1:numel(thermalresults.SolutionTimes)
    resultsByStep = filterByIndex(thermalresults,n);
    model.CellLoad = ...
        cellLoad(Temperature=resultsByStep);
    thermalstressresults = solve(model);
    figure
    pdeplot3D(thermalstressresults.Mesh, ...
              ColorMapData = ...
              thermalstressresults.Displacement.Magnitude, ...
              Deformation =  ...
              thermalstressresults.Displacement)
    title(["Thermal Results at Solution Time = " ...
                             num2str(tlist(n))])
end

Solve Steady-State Thermal Problem

Solve a 3-D steady-state thermal problem.

Create an femodel object for a steady-state thermal problem and include a geometry representing a block.

model = femodel(AnalysisType="thermalSteady", ...
                Geometry="Block.stl");

Plot the block geometry.

pdegplot(model.Geometry, ...
         FaceLabels="on", ...
         FaceAlpha=0.5)
axis equal

Assign material properties.

model.MaterialProperties = ...
    materialProperties(ThermalConductivity=80);

Apply a constant temperature of 100 °C to the left side of the block (face 1) and a constant temperature of 300 °C to the right side of the block (face 3). All other faces are insulated by default.

model.FaceBC(1) = faceBC(Temperature=100);
model.FaceBC(3) = faceBC(Temperature=300);

Mesh the geometry and solve the problem.

model = generateMesh(model);
thermalresults = solve(model)

thermalresults = 
  SteadyStateThermalResults with properties:

    Temperature: [12822x1 double]
     XGradients: [12822x1 double]
     YGradients: [12822x1 double]
     ZGradients: [12822x1 double]
           Mesh: [1x1 FEMesh]

The solver finds the temperatures and temperature gradients at the nodal locations. To access these values, use thermalresults.Temperature, thermalresults.XGradients, and so on. For example, plot temperatures at the nodal locations.

pdeplot3D(thermalresults.Mesh,ColorMapData=thermalresults.Temperature)

Solve Transient Thermal Problem

Solve a 2-D transient thermal problem.

Create a geometry representing a square plate with a diamond-shaped region in its center.

SQ1 = [3; 4; 0; 3; 3; 0; 0; 0; 3; 3];
D1 = [2; 4; 0.5; 1.5; 2.5; 1.5; 1.5; 0.5; 1.5; 2.5];
gd = [SQ1 D1];
sf = 'SQ1+D1';
ns = char('SQ1','D1');
ns = ns';
g = decsg(gd,sf,ns);
pdegplot(g,EdgeLabels="on",FaceLabels="on")
xlim([-1.5 4.5])
ylim([-0.5 3.5])
axis equal

Create an femodel object for transient thermal analysis and include the geometry.

model = femodel(AnalysisType="thermalTransient", ...
                Geometry=g);

For the square region, assign these thermal properties:

• Thermal conductivity is $10\mathrm{W}/\left(\mathrm{m}{\cdot }^{\circ }\mathrm{C}\right)$

• Mass density is $2\mathrm{kg}/{\mathrm{m}}^3$

• Specific heat is $0.1\mathrm{J}/\left({\mathrm{kg}\cdot }^{\circ }\mathrm{C}\right)$

model.MaterialProperties(1) = ...
    materialProperties(ThermalConductivity=10, ...
                       MassDensity=2, ...
                       SpecificHeat=0.1);

For the diamond region, assign these thermal properties:

• Thermal conductivity is $2\mathrm{W}/\left(\mathrm{m}{\cdot }^{\circ }\mathrm{C}\right)$

• Mass density is $1\mathrm{kg}/{\mathrm{m}}^3$

• Specific heat is $0.1\mathrm{J}/\left({\mathrm{kg}\cdot }^{\circ }\mathrm{C}\right)$

model.MaterialProperties(2) = ...
    materialProperties(ThermalConductivity=2, ...
                       MassDensity=1, ...
                       SpecificHeat=0.1);

Assume that the diamond-shaped region is a heat source with a density of $4\mathrm{W}/{\mathrm{m}}^2$.

model.FaceLoad(2) = faceLoad(Heat=4);

Apply a constant temperature of 0 °C to the sides of the square plate.

model.EdgeBC([1 2 7 8]) = edgeBC(Temperature=0);

Set the initial temperature to 0 °C.

model.FaceIC = faceIC(Temperature=0);

Generate the mesh.

model = generateMesh(model);

The dynamics for this problem are very fast. The temperature reaches a steady state in about 0.1 second. To capture the most active part of the dynamics, set the solution time to logspace(-2,-1,10). This command returns 10 logarithmically spaced solution times between 0.01 and 0.1.

tlist = logspace(-2,-1,10);

Solve the equation.

thermalresults = solve(model,tlist);

Plot the solution with isothermal lines by using a contour plot.

T = thermalresults.Temperature;
msh = thermalresults.Mesh;
pdeplot(msh,XYData=T(:,10),Contour="on",ColorMap="hot")

Solve Transient Thermal Problem Using Modal Superposition Method

Solve a transient thermal problem by first obtaining mode shapes for a particular decay range and then using the modal superposition method.

Modal Decomposition

Create a geometry representing a square plate with a diamond-shaped region in its center.

SQ1 = [3; 4; 0; 3; 3; 0; 0; 0; 3; 3];
D1 = [2; 4; 0.5; 1.5; 2.5; 1.5; 1.5; 0.5; 1.5; 2.5];
gd = [SQ1 D1];
sf = 'SQ1+D1';
ns = char('SQ1','D1');
ns = ns';
g = decsg(gd,sf,ns);
pdegplot(g,EdgeLabels="on",FaceLabels="on")
xlim([-1.5 4.5])
ylim([-0.5 3.5])
axis equal

Create an femodel object for modal thermal analysis and include the geometry.

model = femodel(AnalysisType="thermalModal", ...
                Geometry=g);

For the square region, assign these thermal properties:

• Thermal conductivity is $10\mathrm{W}/\left(\mathrm{m}{\cdot }^{\circ }\mathrm{C}\right)$.

• Mass density is $2\mathrm{kg}/{\mathrm{m}}^3$.

• Specific heat is $0.1\mathrm{J}/\left({\mathrm{kg}\cdot }^{\circ }\mathrm{C}\right)$.

model.MaterialProperties(1) = ...
    materialProperties(ThermalConductivity=10, ...
                       MassDensity=2, ...
                       SpecificHeat=0.1);

For the diamond region, assign these thermal properties:

• Thermal conductivity is $2\mathrm{W}/\left(\mathrm{m}{\cdot }^{\circ }\mathrm{C}\right)$.

• Mass density is $1\mathrm{kg}/{\mathrm{m}}^3$.

• Specific heat is $0.1\mathrm{J}/\left({\mathrm{kg}\cdot }^{\circ }\mathrm{C}\right)$.

model.MaterialProperties(2) = ...
    materialProperties(ThermalConductivity=2, ...
                       MassDensity=1, ...
                       SpecificHeat=0.1);

Assume that the diamond-shaped region is a heat source with a density of $4\mathrm{W}/{\mathrm{m}}^2$.

model.FaceLoad(2) = faceLoad(Heat=4);

Apply a constant temperature of 0 °C to the sides of the square plate.

model.EdgeBC([1 2 7 8]) = edgeBC(Temperature=0);

Set the initial temperature to 0 °C.

model.FaceIC = faceIC(Temperature=0);

Generate the mesh.

model = generateMesh(model);

Compute eigenmodes of the model in the decay range [100,10000] $$s^{-1}$$.

RModal = solve(model,DecayRange=[100,10000])

RModal = 
  ModalThermalResults with properties:

    DecayRates: [171x1 double]
    ModeShapes: [1461x171 double]
      ModeType: "EigenModes"
          Mesh: [1x1 FEMesh]

Transient Analysis

Knowing the mode shapes, you can now use the modal superposition method to solve the transient thermal problem. First, switch the model analysis type to thermal transient.

model.AnalysisType = "thermalTransient";

The dynamics for this problem are very fast. The temperature reaches a steady state in about 0.1 second. To capture the most active part of the dynamics, set the solution time to logspace(-2,-1,100). This command returns 100 logarithmically spaced solution times between 0.01 and 0.1.

tlist = logspace(-2,-1,10);

Solve the equation.

Rtransient = solve(model,tlist,ModalResults=RModal);

Plot the solution with isothermal lines by using a contour plot.

msh = Rtransient.Mesh

msh = 
  FEMesh with properties:

             Nodes: [2x1461 double]
          Elements: [6x694 double]
    MaxElementSize: 0.1697
    MinElementSize: 0.0849
     MeshGradation: 1.5000
    GeometricOrder: 'quadratic'

T = Rtransient.Temperature;
pdeplot(msh,XYData=T(:,end),Contour="on", ...
                            ColorMap="hot")

Snapshots for Proper Orthogonal Decomposition

Obtain POD modes of a linear thermal problem using several instances of the transient solution (snapshots).

Create an femodel object for transient thermal analysis and include a unit square geometry in the model.

model = femodel(AnalysisType="thermalTransient", ...
                Geometry=@squareg);

Plot the geometry, displaying edge labels.

pdegplot(model.Geometry,EdgeLabels="on")
xlim([-1.1 1.1])
ylim([-1.1 1.1])

Specify the thermal conductivity, mass density, and specific heat of the material.

model.MaterialProperties = ...
    materialProperties(ThermalConductivity=400, ...
                       MassDensity=1300, ...
                       SpecificHeat=600);

Set the temperature on the right edge to 100.

model.EdgeBC(2) = edgeBC(Temperature=100);

Set an initial value of 0 for the temperature.

model.FaceIC = faceIC(Temperature=0);

Generate a mesh.

model = generateMesh(model);

Solve the model for three different values of heat source and collect snapshots.

tlist = 0:10:600;
snapShotIDs = [1:10 59 60 61];
Tmatrix = [];

heatVariation = [10000 15000 20000];
for q = heatVariation
    model.FaceLoad = faceLoad(Heat=q);
    results = solve(model,tlist);
    Tmatrix = [Tmatrix,results.Temperature(:,snapShotIDs)];
end

Switch the model analysis type to thermal modal.

model.AnalysisType = "thermalModal";

Compute the POD modes.

RModal = solve(model,Snapshots=Tmatrix)

RModal = 
  ModalThermalResults with properties:

          DecayRates: [6x1 double]
          ModeShapes: [1529x6 double]
    SnapshotsAverage: [1529x1 double]
            ModeType: "PODModes"
                Mesh: [1x1 FEMesh]

Solve 2-D Electrostatic Problem

Solve an electromagnetic problem and find the electric potential and field distribution for a 2-D geometry representing a plate with a hole.

Create an femodel object for electrostatic analysis and include a geometry representing a plate with a hole.

model = femodel(AnalysisType="electrostatic",...
                Geometry="PlateHolePlanar.stl");

Plot the geometry with edge labels.

pdegplot(model.Geometry,EdgeLabels="on")

Specify the vacuum permittivity value in the SI system of units.

model.VacuumPermittivity = 8.8541878128E-12;

Specify the relative permittivity of the material.

model.MaterialProperties = ...
    materialProperties(RelativePermittivity=1);

Apply the voltage boundary conditions on the edges framing the rectangle and the circle.

model.EdgeBC(1:4) = edgeBC(Voltage=0);
model.EdgeBC(5) = edgeBC(Voltage=1000);

Specify the charge density for the entire geometry.

model.FaceLoad = faceLoad(ChargeDensity=5E-9);

Generate the mesh.

model = generateMesh(model);

Solve the model.

R = solve(model)

R = 
  ElectrostaticResults with properties:

      ElectricPotential: [1231x1 double]
          ElectricField: [1x1 FEStruct]
    ElectricFluxDensity: [1x1 FEStruct]
                   Mesh: [1x1 FEMesh]

Plot the electric potential and field.

pdeplot(R.Mesh,XYData=R.ElectricPotential, ...
               FlowData=[R.ElectricField.Ex ...
                         R.ElectricField.Ey])
axis equal

Solve 3-D Magnetostatic Problem

Solve a 3-D electromagnetic problem on a geometry representing a plate with a hole in its center. Plot the resulting magnetic potential and field distribution.

Create an femodel object for magnetostatic analysis and include a geometry representing a plate with a hole.

model = femodel(AnalysisType="magnetostatic", ...
                Geometry="PlateHoleSolid.stl");

Plot the geometry.

pdegplot(model.Geometry,FaceLabels="on",FaceAlpha=0.3)

Specify the vacuum permeability value in the SI system of units.

model.VacuumPermeability = 1.2566370614e-6;

Specify the relative permeability of the material.

model.MaterialProperties = ...
    materialProperties(RelativePermeability=5000);

Apply the magnetic potential boundary conditions on the side faces and the face bordering the hole.

model.FaceBC(3:6) = faceBC(MagneticPotential=[0;0;0]); 
model.FaceBC(7) = faceBC(MagneticPotential=[0;0;0.01]);

Specify the current density for the entire geometry.

model.CellLoad = cellLoad(CurrentDensity=[0;0;0.5]);

Generate the mesh.

model = generateMesh(model);

Solve the model.

R = solve(model)

R = 
  MagnetostaticResults with properties:

      MagneticPotential: [1x1 FEStruct]
          MagneticField: [1x1 FEStruct]
    MagneticFluxDensity: [1x1 FEStruct]
                   Mesh: [1x1 FEMesh]

Plot the z-component of the magnetic potential.

pdeplot3D(R.Mesh,ColormapData=R.MagneticPotential.Az)

Plot the magnetic field.

pdeplot3D(R.Mesh,FlowData=[R.MagneticField.Hx ...
                           R.MagneticField.Hy ...
                           R.MagneticField.Hz])

Solve 3-D DC Conduction Problem

Solve a DC conduction problem on a geometry representing a 3-D plate with a hole in its center. Plot the electric potential and the components of the current density.

Create an femodel object for DC conduction analysis and include a geometry representing a plate with a hole.

model = femodel(AnalysisType="dcConduction", ...
                Geometry="PlateHoleSolid.stl");

Plot the geometry.

pdegplot(model.Geometry,FaceLabels="on",FaceAlpha=0.3)

Specify the conductivity of the material.

model.MaterialProperties = ...
    materialProperties(ElectricalConductivity=6e4);

Apply the voltage boundary conditions on the left, right, top, and bottom faces of the plate.

model.FaceBC(3:6) = faceBC(Voltage=0);

Specify the surface current density on the face bordering the hole.

model.FaceLoad(7) = faceLoad(SurfaceCurrentDensity=100);

Generate the mesh.

model = generateMesh(model);

Solve the model.

R = solve(model)

R = 
  ConductionResults with properties:

    ElectricPotential: [4747x1 double]
        ElectricField: [1x1 FEStruct]
       CurrentDensity: [1x1 FEStruct]
                 Mesh: [1x1 FEMesh]

Plot the electric potential.

figure
pdeplot3D(R.Mesh,ColorMapData=R.ElectricPotential)

Plot the x-component of the current density.

figure
pdeplot3D(R.Mesh,ColorMapData=R.CurrentDensity.Jx)
title("x-Component of Current Density")

Plot the y-component of the current density.

figure
pdeplot3D(R.Mesh,ColorMapData=R.CurrentDensity.Jy)
title("y-Component of Current Density")

Plot the z-component of the current density.

figure
pdeplot3D(R.Mesh,ColorMapData=R.CurrentDensity.Jz)
title("z-Component of Current Density")

Use DC Conduction Solution as Current Density for Magnetostatic Analysis

Use a solution obtained by performing a DC conduction analysis to specify current density for a magnetostatic problem.

Create an femodel object for DC conduction analysis and include a geometry representing a plate with a hole.

model = femodel(AnalysisType="dcConduction", ...
                Geometry="PlateHoleSolid.stl");

Plot the geometry.

pdegplot(model.Geometry,FaceLabels="on",FaceAlpha=0.3)

Specify the conductivity of the material.

model.MaterialProperties = ...
    materialProperties(ElectricalConductivity=6e4);

Apply the voltage boundary conditions on the left, right, top, and bottom faces of the plate.

model.FaceBC(3:6) = faceBC(Voltage=0);

Specify the surface current density on the face bordering the hole.

model.FaceLoad(7) = faceLoad(SurfaceCurrentDensity=100);

Generate the mesh.

model = generateMesh(model);

Solve the model.

R = solve(model);

Change the analysis type of the model to magnetostatic.

model.AnalysisType = "magnetostatic";

This model already has a quadratic mesh that you generated for the DC conduction analysis. For a 3-D magnetostatic model, the mesh must be linear. Generate a new linear mesh. The generateMesh function creates a linear mesh by default if the model is 3-D and magnetostatic.

model = generateMesh(model);

Specify the vacuum permeability value in the SI system of units.

model.VacuumPermeability = 1.2566370614e-6;

Specify the relative permeability of the material.

model.MaterialProperties = ...
    materialProperties(RelativePermeability=5000);

Apply the magnetic potential boundary conditions on the side faces and the face bordering the hole.

model.FaceBC(3:6) = faceBC(MagneticPotential=[0;0;0]);
model.FaceBC(7) = faceBC(MagneticPotential=[0;0;0.01]);

Specify the current density for the entire geometry using the DC conduction solution.

model.CellLoad = cellLoad(CurrentDensity=R);

Solve the problem.

Rmagnetostatic = solve(model);

Plot the x- and z-components of the magnetic potential.

pdeplot3D(Rmagnetostatic.Mesh, ...
          ColormapData=Rmagnetostatic.MagneticPotential.Ax)

pdeplot3D(Rmagnetostatic.Mesh, ...
          ColormapData=Rmagnetostatic.MagneticPotential.Az)

Solve 2-D Magnetostatic Problem with Permanent Magnet

Solve a magnetostatic problem of a copper square with a permanent neodymium magnet in its center.

Create the unit square geometry with a circle in its center.

L = 0.8;
r = 0.25;
sq = [3 4 -L L L -L -L -L L L]';
circ = [1 0 0 r 0 0 0 0 0 0]';
gd = [sq,circ];
sf = "sq + circ";
ns = char('sq','circ');
ns = ns';
g = decsg(gd,sf,ns);

Plot the geometry with the face and edge labels.

pdegplot(g,FaceLabels="on",EdgeLabels="on")

Create an femodel object for magnetostatic analysis and include the geometry in the model.

model = femodel(AnalysisType="magnetostatic", ...
                Geometry=g);

Specify the vacuum permeability value in the SI system of units.

model.VacuumPermeability = 1.2566370614e-6;

Specify the relative permeability of the copper for the square.

model.MaterialProperties(1) = ...
    materialProperties(RelativePermeability=1);

Specify the relative permeability of the neodymium for the circle.

model.MaterialProperties(2) = ...
    materialProperties(RelativePermeability=1.05);

Specify the magnetization magnitude for the neodymium magnet.

M = 1e6;

Specify magnetization on the circular face in the positive x-direction. Magnetization for a 2-D model is a column vector of two elements.

dir = [1;0];
model.FaceLoad(2) = faceLoad(Magnetization=M*dir);

Apply the magnetic potential boundary conditions on the edges framing the square.

model.EdgeBC(1:4) = edgeBC(MagneticPotential=0);

Generate the mesh with finer meshing near the edges of the circle.

model = generateMesh(model,Hedge={5:8,0.007});
figure
pdemesh(model)

Solve the problem, and find the resulting magnetic fields B and H. Here, $\mathit{B}=\mu \mathit{H}+{\mu }_0\mathit{M}$, where $\mu$ is the absolute magnetic permeability of the material, ${\mu }_0$ is the vacuum permeability, and $\mathit{M}$ is the magnetization.

R = solve(model);
Bmag = sqrt(R.MagneticFluxDensity.Bx.^2 + R.MagneticFluxDensity.By.^2);
Hmag = sqrt(R.MagneticField.Hx.^2 + R.MagneticField.Hy.^2);

Plot the magnetic field B.

figure
pdeplot(R.Mesh,XYData=Bmag, ...
               FlowData=[R.MagneticFluxDensity.Bx ...
                         R.MagneticFluxDensity.By])

Plot the magnetic field H.

figure
pdeplot(R.Mesh,XYData=Hmag, ...
               FlowData=[R.MagneticField.Hx R.MagneticField.Hy])

Solve 2-D Harmonic Electromagnetic Problem

For an electromagnetic harmonic analysis problem, find the x- and y-components of the electric field. Solve the problem on a domain consisting of a square with a circular hole.

For the geometry, define a circle in a square, place them in one matrix, and create a set formula that subtracts the circle from the square.

SQ = [3,4,-5,-5,5,5,-5,5,5,-5]';
C = [1,0,0,1]';
C = [C;zeros(length(SQ) - length(C),1)];
gm = [SQ,C];
sf = 'SQ-C';

Create the geometry.

ns = char('SQ','C');
ns = ns';
g = decsg(gm,sf,ns);

Create an femodel object for electromagnetic harmonic analysis with an electric field type. Include the geometry in the model.

model = femodel(AnalysisType="electricHarmonic", ...
                Geometry=g);

Plot the geometry with the edge labels.

pdegplot(model.Geometry,EdgeLabels="on")
xlim([-5.5 5.5])
ylim([-5.5 5.5])

Specify the vacuum permittivity and permeability values as 1.

model.VacuumPermittivity = 1;
model.VacuumPermeability = 1;

Specify the relative permittivity, relative permeability, and conductivity of the material.

model.MaterialProperties = ...
    materialProperties(RelativePermittivity=1, ...
                       RelativePermeability=1, ...
                       ElectricalConductivity=0);

Apply the absorbing boundary condition with a thickness of 2 on the edges of the square. Use the default attenuation rate for the absorbing region.

ffbc = farFieldBC(Thickness=2);
model.EdgeBC(1:4) = edgeBC(FarField=ffbc);

Specify an electric field on the edges of the hole.

E = @(location,state) [1;0]*exp(-1i*2*pi*location.y); 
model.EdgeBC(5:8) = edgeBC(ElectricField=E);

Generate a mesh.

model = generateMesh(model,Hmax=1/2^3);

Solve the model for a frequency of $2\pi$.

result = solve(model,2*pi);

Plot the real part of the x-component of the resulting electric field.

figure
pdeplot(result.Mesh,XYData=real(result.ElectricField.Ex));
title("Real Part of x-Component of Electric Field")

Plot the real part of the y-component of the resulting electric field.

figure
pdeplot(result.Mesh,XYData=real(result.ElectricField.Ey));
title("Real Part of y-Component of Electric Field")

Input Arguments

fem — Finite element analysis model

femodel object

Finite element analysis model, specified as an femodel object. The model contains information about a finite element problem: analysis type, geometry, material properties, boundary conditions, loads, initial conditions, and other parameters. Depending on the analysis type, it represents a structural, thermal, or electromagnetic problem.

Example: model = femodel(AnalysisType = "structuralStatic")

structuralStatic — Static structural analysis model

StructuralModel object

Static structural analysis model, specified as a StructuralModel object. The model contains the geometry, mesh, structural properties of the material, body loads, boundary loads, and boundary conditions.

Example: structuralmodel = createpde("structural","static-solid")

structuralTransient — Transient structural analysis model

StructuralModel object

Transient structural analysis model, specified as a StructuralModel object. The model contains the geometry, mesh, structural properties of the material, body loads, boundary loads, and boundary conditions.

Example: structuralmodel = createpde("structural","transient-solid")

structuralFrequencyResponse — Frequency response analysis structural model

StructuralModel object

Frequency response analysis structural model, specified as a StructuralModel object. The model contains the geometry, mesh, structural properties of the material, body loads, boundary loads, and boundary conditions.

Example: structuralmodel = createpde("structural","frequency-solid")

structuralModal — Modal analysis structural model

StructuralModel object

Modal analysis structural model, specified as a StructuralModel object. The model contains the geometry, mesh, structural properties of the material, body loads, boundary loads, and boundary conditions.

Example: structuralmodel = createpde("structural","modal-solid")

tlist — Solution times for structural or thermal transient analysis

real vector

Solution times for structural or thermal transient analysis, specified as a real vector of monotonically increasing or decreasing values.

Example: 0:20

Data Types: double

flist — Solution frequencies for frequency response structural analysis

real vector

Solution frequencies for a frequency response structural analysis, specified as a real vector of monotonically increasing or decreasing values.

Example: linspace(0,4000,150)

Data Types: double

[omega1,omega2] — Frequency range for structural modal analysis

vector of two elements

Frequency range for a structural modal analysis, specified as a vector of two elements. Define omega1 as slightly lower than the lowest expected frequency and omega2 as slightly higher than the highest expected frequency. For example, if the lowest expected frequency is zero, then use a small negative value for omega1.

Example: [-0.1,1000]

Data Types: double

structuralModalR — Modal analysis results for structural model

ModalStructuralResults object

Modal analysis results for a structural model, specified as a ModalStructuralResults object.

Example: structuralModalR = solve(structuralmodel,FrequencyRange=[0,1e6])

thermalSteadyState — Steady-state thermal analysis model

ThermalModel object

Steady-state thermal analysis model, specified as a ThermalModel object. ThermalModel contains the geometry, mesh, thermal properties of the material, internal heat source, Stefan-Boltzmann constant, boundary conditions, and initial conditions.

Example: thermalmodel = createpde("thermal","steadystate")

thermalTransient — Transient thermal analysis model

ThermalModel object

Transient thermal analysis model, specified as a ThermalModel object. ThermalModel contains the geometry, mesh, thermal properties of the material, internal heat source, Stefan-Boltzmann constant, boundary conditions, and initial conditions.

thermalModal — Modal thermal analysis model

ThermalModel object

Modal thermal analysis model, specified as a ThermalModel object. ThermalModel contains the geometry, mesh, thermal properties of the material, internal heat source, Stefan-Boltzmann constant, boundary conditions, and initial conditions.

[lambda1,lambda2] — Decay range for modal thermal analysis

vector of two elements

Decay range for modal thermal analysis, specified as a vector of two elements. The solve function solves a modal thermal analysis model for all modes in the decay range.

Data Types: double

Tmatrix — Thermal model solution snapshots

matrix

Thermal model solution snapshots, specified as a matrix.

Data Types: double

thermalModalR — Modal analysis results for thermal model

ModalThermalResults object

Modal analysis results for a thermal model, specified as a ModalThermalResults object.

Example: thermalModalR = solve(thermalmodel,DecayRange=[0,1000])

z — Modal damping ratio

nonnegative number | function handle

Modal damping ratio, specified as a nonnegative number or a function handle. Use a function handle when each mode has its own damping ratio. The function must accept a vector of natural frequencies as an input argument and return a vector of corresponding damping ratios. It must cover the full frequency range for all modes used for modal solution. For details, see Modal Damping Depending on Frequency.

Data Types: double | function_handle

emagmodel — Electromagnetic model for electrostatic, magnetostatic, or DC conduction analysis

ElectromagneticModel object

Electromagnetic model for electrostatic, magnetostatic, or DC conduction analysis, specified as an ElectromagneticModel object. The model contains the geometry, mesh, material properties, electromagnetic sources, and boundary conditions.

Example: emagmodel = createpde("electromagnetic","magnetostatic")

omega — Solution frequencies for harmonic electromagnetic analysis

nonnegative number | vector of nonnegative numbers

Solution frequencies for a harmonic electromagnetic analysis, specified as a nonnegative number or a vector of nonnegative numbers.

Data Types: double

Output Arguments

results — Structural, thermal, or electromagnetic analysis results

StaticStructuralResults object | TransientStructuralResults object | FrequencyStructuralResults object | ModalStructuralResults object | SteadyStateThermalResults object | TransientThermalResults object | ModalThermalResults object | ElectrostaticResults object | MagnetostaticResults object | ConductionResults object | HarmonicResults object

Structural, thermal, or electromagnetic analysis results, returned as a StaticStructuralResults, TransientStructuralResults, FrequencyStructuralResults, ModalStructuralResults, SteadyStateThermalResults, TransientThermalResults, ModalThermalResults, ElectrostaticResults, MagnetostaticResults, ConductionResults, or HarmonicResults object.

structuralStaticResults — Static structural analysis results

StaticStructuralResults object

Static structural analysis results, returned as a StaticStructuralResults object.

structuralTransientResults — Transient structural analysis results

TransientStructuralResults object

Transient structural analysis results, returned as a TransientStructuralResults object.

structuralFrequencyResponseResults — Frequency response structural analysis results

FrequencyStructuralResults object

Frequency response structural analysis results, returned as a FrequencyStructuralResults object.

structuralModalResults — Modal structural analysis results

ModalStructuralResults object

Modal structural analysis results, returned as a ModalStructuralResults object.

thermalSteadyStateResults — Steady-state thermal analysis results

SteadyStateThermalResults object

Steady-state thermal analysis results, returned as a SteadyStateThermalResults object.

thermalTransientResults — Transient thermal analysis results

TransientThermalResults object

Transient thermal analysis results, returned as a TransientThermalResults object.

thermalModalResults — Modal thermal analysis results

ModalThermalResults object

Modal thermal analysis results, returned as a ModalThermalResults object.

emagStaticResults — Electrostatic, magnetostatic or DC conduction analysis results

ElectrostaticResults object | MagnetostaticResults object | ConductionResults object

Electrostatic, magnetostatic, or DC conduction analysis results, returned as an ElectrostaticResults, MagnetostaticResults, or ConductionResults object.

emagHarmonicResults — Harmonic electromagnetic analysis results

HarmonicResults object

Harmonic electromagnetic analysis results, returned as a HarmonicResults object.

Tips

• When you use modal analysis results to solve a transient structural dynamics model, the modalresults argument must be created in Partial Differential Equation Toolbox™ from R2019a or newer.

• For a frequency response model with damping, the results are complex. Use functions such as abs and angle to obtain real-valued results, such as the magnitude and phase.

Version History

Introduced in R2017a

R2023a: Finite element model

The solver accepts the femodel object that defines structural mechanics, thermal, and electromagnetic problems.

R2022b: DC conduction and permanent magnets

You can now solve stationary current distribution in conductors due to applied voltage. You also can solve electromagnetic problems accounting for magnetization of materials.

R2022a: Harmonic electromagnetic analysis

You can now solve 2-D and 3-D time-harmonic Maxwell’s equations (the Helmholtz equation).

R2022a: Reduced-order modeling for thermal analysis

You can now compute modes of a thermal model using eigenvalue or proper orthogonal decomposition. You also can speed up computations for a transient thermal model by using the computed modes.

R2021b: 3-D electrostatic and magnetostatic problems

You can now solve 3-D electrostatic and magnetostatic problems.

R2021a: 2-D electrostatic and magnetostatic problems

You can now solve 2-D electrostatic and magnetostatic problems.

R2020a: Axisymmetric analysis

You can now solve axisymmetric structural and thermal problems. Axisymmetric analysis simplifies 3-D thermal problems to 2-D using their symmetry around the axis of rotation.

R2019b: Frequency response structural analysis

You can now solve frequency response structural problems and find displacement, velocity, acceleration, and solution frequencies at nodal locations of the mesh. To speed up computations, you can use modal analysis results for frequency response analysis. The ModalResults argument triggers the solve function to use the modal superposition method.

R2019b: Lanczos algorithm for structural modal analysis problems

You can now specify the maximum number of Lanczos shifts and the block size for block Lanczos recurrence by using the SolverOptions property of StructuralModel. For details, see PDESolverOptions Properties.

R2019a: Modal superposition method for transient structural analysis

The new ModalResults argument triggers the solve function to switch to the modal transient solver instead of using the direct integration approach.

R2018b: Thermal stress

The solver now solves accounts for mechanical and thermal effects when solving a static structural analysis model. The function returns a displacement, stress, strain, and von Mises stress induced by both mechanical and thermal loads.

R2018a: Transient and modal structural analyses

You can now solve dynamic linear elasticity problems and find displacement, velocity, and acceleration at nodal locations of the mesh.

You also can solve modal analysis problems and find natural frequencies and mode shapes of a structure. When solving a modal analysis model, the solver requires a frequency range parameter and returns the modal solution in that frequency range.

R2017b: Static structural analysis

You can now solve static linear elasticity problems and find displacement, stress, strain, and von Mises stress at nodal locations of the mesh.