interpolateVonMisesStress
Interpolate von Mises stress at arbitrary spatial locations
Syntax
Description
returns the interpolated von Mises stress values at the 2-D points specified in
intrpVMStress
= interpolateVonMisesStress(structuralresults
,xq
,yq
)xq
and yq
. For transient and frequency
response structural problems, interpolateVonMisesStress
interpolates von Mises stress for all time or frequency steps, respectively.
uses the 3-D points specified in intrpVMStress
= interpolateVonMisesStress(structuralresults
,xq
,yq
,zq
)xq
, yq
, and
zq
.
uses the points specified in intrpVMStress
= interpolateVonMisesStress(structuralresults
,querypoints
)querypoints
.
Examples
Interpolate von Mises Stress 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);
Switch the model type to plane-strain.
model.PlanarType = "planeStrain";
Plot the geometry.
pdegplot(model.Geometry,EdgeLabels="on")
xlim([-1.1 1.1])
ylim([-1.1 1.1])
Specify Young's modulus and Poisson's ratio.
model.MaterialProperties = ... materialProperties(PoissonsRatio=0.3, ... YoungsModulus=210E3);
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 von Mises stress to the grid.
v = linspace(-1,1,151); [X,Y] = meshgrid(v); intrpVMStress = interpolateVonMisesStress(R,X,Y);
Reshape the von Mises stress to the shape of the grid and plot it.
VMStress = reshape(intrpVMStress,size(X));
p = pcolor(X,Y,VMStress);
p.EdgeColor="none";
colorbar
Interpolate Von Mises Stress for 3-D Static Structural Analysis Problem
Analyze a bimetallic cable under tension, and interpolate the von Mises stress 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
object 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 von Mises stress and plot the result.
IntrpVMStress = interpolateVonMisesStress(R,X,Y,Z); surf(X,Y,reshape(IntrpVMStress,size(X)))
Alternatively, you can specify the grid by using a matrix of query points.
querypoints = [X(:),Y(:),Z(:)]';
IntrpVMStress = ...
interpolateVonMisesStress(R,querypoints);
surf(X,Y,reshape(IntrpVMStress,size(X)))
Interpolate von Mises Stress for 3-D Structural Dynamic Problem
Interpolate the von Mises stress 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 von Mises stress at the geometric center of the beam.
coordsMidSpan = [0;0;0.005]; VMStress = interpolateVonMisesStress(R,coordsMidSpan);
Plot the von Mises stress at the geometric center of the beam.
plot(R.SolutionTimes,VMStress)
title("von Mises Stress 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.
interpolateVonMisesStress
evaluates the von Mises
stress 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.
interpolateVonMisesStress
converts query points to
column vectors xq(:)
, yq(:)
, and (if
present) zq(:)
. The function returns von Mises stress as
a column vector of the same size as the query point 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 intrpVMStress =
reshape(intrpVMStress,size(xq))
.
Data Types: double
yq
— y-coordinate query points
real array
y-coordinate query points, specified as a real array.
interpolateVonMisesStress
evaluates the von Mises
stress 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, interpolateVonMisesStress
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.
interpolateVonMisesStress
evaluates the von Mises
stress 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,
interpolateVonMisesStress
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. interpolateVonMisesStress
evaluates the von Mises stress 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
intrpVMStress
— von Mises stress at query points
column vector
von Mises stress at the query points, returned as a column vector.
For query points that are outside the geometry,
intrpVMStress
= NaN
.
Version History
Introduced in R2017bR2019b: Support for frequency response structural problems
For frequency response structural problems,
interpolateVonMisesStress
interpolates von Mises stress for
all frequency steps.
R2018a: Support for transient structural problems
For transient structural problems, interpolateVonMisesStress
interpolates von Mises stress for all time steps.
MATLAB Command
You clicked a link that corresponds to this MATLAB command:
Run the command by entering it in the MATLAB Command Window. Web browsers do not support MATLAB commands.
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)