interpolateStrain

Interpolate strain at arbitrary spatial locations

Syntax

intrpStrain = interpolateStrain(structuralresults,xq,yq)

intrpStrain = interpolateStrain(structuralresults,xq,yq,zq)

intrpStrain = interpolateStrain(structuralresults,querypoints)

Description

intrpStrain = interpolateStrain(structuralresults,xq,yq) returns the interpolated strain values at the 2-D points specified in xq and yq. For transient and frequency-response structural problems, interpolateStrain interpolates strain for all time or frequency steps, respectively.

intrpStrain = interpolateStrain(structuralresults,xq,yq,zq) uses the 3-D points specified in xq, yq, and zq.

intrpStrain = interpolateStrain(structuralresults,querypoints) uses the points specified in querypoints.

Examples

Interpolate Strain for Plane-Strain Problem

Create an femodel object for static structural analysis and include a unit square geometry into the model.

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

Plot the geometry.

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

Switch the problem type to plane-strain.

model.PlanarType = "planeStrain";

Specify Young's modulus and Poisson's ratio.

model.MaterialProperties = ...
    materialProperties(YoungsModulus=210E3, ...
                       PoissonsRatio=0.3);

Specify the x-component of the enforced displacement for edge 1.

model.EdgeBC(1) = edgeBC(XDisplacement=0.001);

Specify that edge 3 is a fixed boundary.

model.EdgeBC(3) = edgeBC(Constraint="fixed");

Generate a mesh and solve the problem.

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

Create a grid and interpolate the x- and y-components of the normal strain to the grid.

v = linspace(-1,1,101);
[X,Y] = meshgrid(v);
intrpStrain = interpolateStrain(R,X,Y);

Reshape the x-component of the normal strain to the shape of the grid and plot it.

exx = reshape(intrpStrain.exx,size(X));
px = pcolor(X,Y,exx);
px.EdgeColor="none";
colorbar

Reshape the y-component of the normal strain to the shape of the grid and plot it.

eyy = reshape(intrpStrain.eyy,size(Y));
figure
py = pcolor(X,Y,eyy);
py.EdgeColor="none";
colorbar

Interpolate Strain for 3-D Static Structural Analysis Problem

Analyze a bimetallic cable under tension, and interpolate strain on a cross-section of the cable.

Create and plot a geometry representing a bimetallic cable.

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

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

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]

Define the coordinates of a midspan cross-section of the cable.

[X,Y] = meshgrid(linspace(-0.015,0.015,50));
Z = ones(size(X))*0.025;

Interpolate the strain and plot the result.

intrpStrain = interpolateStrain(R,X,Y,Z);
surf(X,Y,reshape(intrpStrain.ezz,size(X)))

Alternatively, you can specify the grid by using a matrix of query points.

querypoints = [X(:),Y(:),Z(:)]';
intrpStrain = interpolateStrain(R,querypoints);
surf(X,Y,reshape(intrpStrain.ezz,size(X)))

Interpolate Strain for 3-D Structural Dynamic Problem

Interpolate the strain at the geometric center of a beam under a harmonic excitation.

Create and plot a beam geometry.

gm = multicuboid(0.06,0.005,0.01);
pdegplot(gm,FaceLabels="on",FaceAlpha=0.5)
view(50,20)

Create an femodel object for transient structural analysis and include the geometry into the model.

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);

Fix one end of the beam.

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

Apply a sinusoidal displacement along the y-direction on the end opposite the fixed end of the beam.

yDisplacementFunc = ...
@(location,state) ones(size(location.y))*1E-4*sin(50*state.time);
model.FaceBC(3) = faceBC(YDisplacement=yDisplacementFunc);

Generate a mesh.

model = generateMesh(model,Hmax=0.01);

Specify the zero initial displacement and velocity.

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

Solve the problem.

tlist = 0:0.002:0.2;
R = solve(model,tlist);

Interpolate the strain at the geometric center of the beam.

coordsMidSpan = [0;0;0.005];
intrpStrain = interpolateStrain(R,coordsMidSpan);

Plot the normal strain at the geometric center of the beam.

plot(R.SolutionTimes,intrpStrain.exx)
title("X-Direction Normal Strain at Beam Center")

Input Arguments

structuralresults — Solution of structural analysis problem

StaticStructuralResults object | TransientStructuralResults object | FrequencyStructuralResults object

Solution of the structural analysis problem, specified as a StaticStructuralResults, TransientStructuralResults, or FrequencyStructuralResults object. Create structuralresults by using the solve function.

xq — x-coordinate query points

real array

x-coordinate query points, specified as a real array. interpolateStrain evaluates the strains at the 2-D coordinate points [xq(i),yq(i)] or at the 3-D coordinate points [xq(i),yq(i),zq(i)]. Therefore, xq, yq, and (if present) zq must have the same number of entries.

interpolateStrain converts query points to column vectors xq(:), yq(:), and (if present) zq(:). The function returns strains as an FEStruct object with the properties containing vectors of the same size as these column vectors. To ensure that the dimensions of the returned solution are consistent with the dimensions of the original query points, use the reshape function. For example, use intrpStrain = reshape(intrpStrain.exx,size(xq)).

Data Types: double

yq — y-coordinate query points

real array

y-coordinate query points, specified as a real array. interpolateStrain evaluates the strains at the 2-D coordinate points [xq(i),yq(i)] or at the 3-D coordinate points [xq(i),yq(i),zq(i)]. Therefore, xq, yq, and (if present) zq must have the same number of entries. Internally, interpolateStrain converts the query points to the column vector yq(:).

Data Types: double

zq — z-coordinate query points

real array

z-coordinate query points, specified as a real array. interpolateStrain evaluates the strains at the 3-D coordinate points [xq(i),yq(i),zq(i)]. Therefore, xq, yq, and zq must have the same number of entries. Internally, interpolateStrain converts the query points to the column vector zq(:).

Data Types: double

querypoints — Query points

real matrix

Query points, specified as a real matrix with either two rows for 2-D geometry or three rows for 3-D geometry. interpolateStrain evaluates the strains at the coordinate points querypoints(:,i), so each column of querypoints contains exactly one 2-D or 3-D query point.

Example: For 2-D geometry, querypoints = [0.5,0.5,0.75,0.75; 1,2,0,0.5]

Data Types: double

Output Arguments

intrpStrain — Strains at query points

FEStruct object

Strains at the query points, returned as an FEStruct object with the properties representing spatial components of strain at the query points. For query points that are outside the geometry, intrpStrain returns NaN. Properties of an FEStruct object are read-only.

Version History

Introduced in R2017b

R2019b: Support for frequency response structural problems

For frequency response structural problems, interpolateStrain interpolates strain for all frequency steps.

R2018a: Support for transient structural problems

For transient structural problems, interpolateStrain interpolates strain for all time steps.