interpolateStrain
Interpolate strain at arbitrary spatial locations
Syntax
Description
returns the interpolated strain values at the 2-D points specified in
intrpStrain
= interpolateStrain(structuralresults
,xq
,yq
)xq
and yq
. For transient and
frequency-response structural problems, interpolateStrain
interpolates strain for all time or frequency steps, respectively.
uses the 3-D points specified in intrpStrain
= interpolateStrain(structuralresults
,xq
,yq
,zq
)xq
, yq
, and
zq
.
uses the points specified in intrpStrain
= interpolateStrain(structuralresults
,querypoints
)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 R2017bR2019b: 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.
MATLAB-Befehl
Sie haben auf einen Link geklickt, der diesem MATLAB-Befehl entspricht:
Führen Sie den Befehl durch Eingabe in das MATLAB-Befehlsfenster aus. Webbrowser unterstützen keine MATLAB-Befehle.
Select a Web Site
Choose a web site to get translated content where available and see local events and offers. Based on your location, we recommend that you select: .
You can also select a web site from the following list:
How to Get Best Site Performance
Select the China site (in Chinese or English) for best site performance. Other MathWorks country sites are not optimized for visits from your location.
Americas
- América Latina (Español)
- Canada (English)
- United States (English)
Europe
- Belgium (English)
- Denmark (English)
- Deutschland (Deutsch)
- España (Español)
- Finland (English)
- France (Français)
- Ireland (English)
- Italia (Italiano)
- Luxembourg (English)
- Netherlands (English)
- Norway (English)
- Österreich (Deutsch)
- Portugal (English)
- Sweden (English)
- Switzerland
- United Kingdom (English)