structuralBC
Specify boundary conditions for structural model
Domain-specific structural workflow is not recommended. New features might not be compatible with this workflow. For help migrating your existing code to the unified finite element workflow, see Migration from Domain-Specific to Unified Workflow.
Syntax
Description
Standard Boundary Constraints and Displacements
structuralBC(
specifies one of the standard structural boundary constraints. Here,
structuralmodel,RegionType,RegionID,"Constraint",Cval)Cval can be "fixed",
"free", "roller", or
"symmetric". The default value is
"free".
Avoid using "symmetric" for transient and modal analysis,
since the symmetric constraint can prevent the participation of some structural
modes.
structuralBC(
enforces displacement on the boundary of type structuralmodel,RegionType,RegionID,"Displacement",Dval)RegionType
with RegionID ID numbers.
structuralBC(
specifies the x-, y-, and z-components of the enforced displacement.structuralmodel,RegionType,RegionID,"XDisplacement",XDval,"YDisplacement",YDval,"ZDisplacement",ZDval)
structuralBC does not require you to specify all three
components. Depending on your structural analysis problem, you can specify one
or more components by picking the corresponding arguments and omitting
others.
structuralBC(
specifies the r- and z-components of the enforced displacement for an
axisymmetric model. The radial component (r-component) must be zero on the axis
of rotation.structuralmodel,RegionType,RegionID,"RDisplacement",RDval,"ZDisplacement",ZDval)
structuralBC does not require you to specify both
components.
Harmonic, Rectangular, Triangular, and Trapezoidal Displacement Pulses
structuralBC(specifies
the form and duration of the time-varying value of the x-component of the
enforced displacement. You can also specify the form and duration of the other
components of the displacement as follows:structuralmodel,RegionType,RegionID,"XDisplacement",XDval,Name,Value)
structuralBC(...,"YDisplacement",for the y-component.YDval,Name,Value)structuralBC(...,"ZDisplacement",for the z-component. Use this syntax for a 3-D or axisymmetric model.ZDval,Name,Value)structuralBC(...,"RDisplacement",for the radial component in an axisymmetric model.RDval,Name,Value)
Multipoint Constraint
structuralBC(
sets the multipoint constraint using all degrees of freedom on the combination
of geometric regions specified by structuralmodel,RegionType,RegionID,"Constraint","multipoint")RegionType and
RegionID. The reference location for the constraint is
the geometric center of all nodes on the combination of all specified geometric
regions.
This syntax is required if you intend to use results obtained with the model
order reduction technique in the Simscape™
Multibody™
Reduced Order Flexible Solid block. Simscape models expect the connections at all joints to have six degrees of
freedom, while Partial Differential Equation Toolbox™ uses two or three degrees of freedom at each node. Setting a
multipoint constraint ensures that all nodes and all degrees of freedom for the
specified geometric regions have a rigid constraint with the geometric center of
all specified geometric regions altogether as the reference point. The reference
location has six degrees of freedom.
For better performance, specify geometric regions with a minimal number of nodes. For example, use a set of edges instead of using a face, and a set of vertices instead of using an edge.
structuralBC(___,"Reference",
specifies the reference point for the multipoint constraint instead of using the
geometric center of all specified regions as a reference point. Coords)
Use this syntax with the input arguments from the previous syntax.
Sparse Linear Models for Use with Control System Toolbox
structuralBC(___,"Label",
adds a label for the structural boundary condition to be used by the labeltext)linearizeInput function. This function lets you pass boundary
conditions to the linearize function that extracts sparse linear models for use
with Control System Toolbox™.
Vectorized Evaluation for Function Handles
structuralBC(___,"Vectorized","on") uses
vectorized function evaluation when you pass a function handle as an argument.
If your function handle computes in a vectorized fashion, then using this
argument saves time. See Vectorization. For details on this
evaluation, see Nonconstant Boundary Conditions.
Use this syntax with any of the input arguments from previous syntaxes.
Structural Boundary Condition Object
bc = structuralBC(___)
Examples
Apply Fixed Boundaries and Specify Surface Traction
Apply fixed boundaries and traction on two ends of a bimetallic cable.
Create a structural model.
structuralModel = createpde("structural","static-solid");
Create nested cylinders to model a bimetallic cable.
gm = multicylinder([0.01,0.015],0.05);
Assign the geometry to the structural model and plot the geometry.
structuralModel.Geometry = gm; pdegplot(structuralModel,"CellLabels","on", ... "FaceLabels","on", ... "FaceAlpha",0.4)
For each metal, specify Young's modulus and Poisson's ratio.
structuralProperties(structuralModel,"Cell",1,"YoungsModulus",110E9, ... "PoissonsRatio",0.28); structuralProperties(structuralModel,"Cell",2,"YoungsModulus",210E9, ... "PoissonsRatio",0.3);
Specify that faces 1 and 4 are fixed boundaries.
structuralBC(structuralModel,"Face",[1,4],"Constraint","fixed")
ans =
StructuralBC with properties:
RegionType: 'Face'
RegionID: [1 4]
Vectorized: 'off'
Boundary Constraints and Enforced Displacements
Displacement: []
XDisplacement: []
YDisplacement: []
ZDisplacement: []
Constraint: "fixed"
Radius: []
Reference: []
Label: []
Boundary Loads
Force: []
SurfaceTraction: []
Pressure: []
TranslationalStiffness: []
Label: []
Specify the surface traction for faces 2 and 5.
structuralBoundaryLoad(structuralModel, ... "Face",[2,5], ... "SurfaceTraction",[0;0;100])
ans =
StructuralBC with properties:
RegionType: 'Face'
RegionID: [2 5]
Vectorized: 'off'
Boundary Constraints and Enforced Displacements
Displacement: []
XDisplacement: []
YDisplacement: []
ZDisplacement: []
Constraint: []
Radius: []
Reference: []
Label: []
Boundary Loads
Force: []
SurfaceTraction: [3x1 double]
Pressure: []
TranslationalStiffness: []
Label: []
Specify Displacements
Create a structural model.
structuralModel = createpde("structural","static-solid");
Create a block geometry.
gm = multicuboid(0.2,0.1,0.05);
Assign the geometry to the structural model and plot the geometry.
structuralModel.Geometry = gm; pdegplot(structuralModel,"FaceLabels","on","FaceAlpha",0.5)
Specify Young's modulus, Poisson's ratio, and the mass density.
structuralProperties(structuralModel,"YoungsModulus",74e9,... "PoissonsRatio",0.42,... "MassDensity",19.29e3);
Specify the gravity load on the beam.
structuralBodyLoad(structuralModel, ... "GravitationalAcceleration",[0;0;-9.8]);
Specify that face 5 is a fixed boundary.
structuralBC(structuralModel,"Face",5,"Constraint","fixed");
Specify z-displacement on face 3 of the model. By leaving the x- and y-displacements unspecified, you enable face 3 to move in the x- and y-directions.
structuralBC(structuralModel,"Face",3,"ZDisplacement",0.0001);
Generate a mesh and solve the model.
generateMesh(structuralModel); R = solve(structuralModel);
Plot the deformed shape with the x-component of normal stress.
pdeplot3D(structuralModel,"ColorMapData",R.Stress.sxx, ... "Deformation",R.Displacement)
Now specify all three displacements on the same face. Here, the z-displacement is the same, but the x- and y-displacements are both zero. Face 3 cannot move in the x- and y-directions.
structuralBC(structuralModel,"Face",3, ... "Displacement",[0;0;0.0001]); R = solve(structuralModel); pdeplot3D(structuralModel,"ColorMapData",R.Stress.sxx, ... "Deformation",R.Displacement)
Thus, specifying "Displacement",[0;0;0.0001] is equivalent to specifying "XDisplacement",0,"YDisplacement",0,"ZDisplacement",0.0001.
structuralBC(structuralModel,"Face",3,"XDisplacement",0, ... "YDisplacement",0, ... "ZDisplacement",0.0001); R = solve(structuralModel); pdeplot3D(structuralModel,"ColorMapData",R.Stress.sxx, ... "Deformation",R.Displacement)
Static Analysis of Spinning Disk with Press-Fit at Hub
Analyze a spinning disk with radial compression at the hub due to press-fit. The inner radius of the disk is 0.05, and the outer radius is 0.2. The thickness of the disk is 0.05 with an interference fit of 50E-6. For this analysis, simplify the 3-D axisymmetric model to a 2-D model.
Create a static structural analysis model for solving an axisymmetric problem.
structuralmodel = createpde("structural","static-axisymmetric");
The 2-D model is a rectangular strip whose x-dimension extends from the hub to the outer surface, and whose y-dimension extends over the height of the disk. Create the geometry by specifying the coordinates of the strip's four corners. For axisymmetric models, the toolbox assumes that the axis of rotation is the vertical axis passing through r = 0, which is equivalent to x = 0.
g = decsg([3 4 0.05 0.2 0.2 0.05 -0.025 -0.025 0.025 0.025]');
Include the geometry in the model.
geometryFromEdges(structuralmodel,g);
Plot the geometry with the edge and vertex labels.
figure pdegplot(structuralmodel,"EdgeLabels","on","VertexLabels","on") xlim([0 0.3]) ylim([-0.05 0.05])
Specify Young's modulus, Poisson's ratio, and the mass density.
structuralProperties(structuralmodel,"YoungsModulus",210e9, ... "PoissonsRatio",0.28, ... "MassDensity",7700);
Apply centrifugal load due to spinning of the disk. Assume that the disk is spinning at 104.7 rad/s.
structuralBodyLoad(structuralmodel,"AngularVelocity",104.7);Apply radial displacement at the hub of the disk to model press-fit.
structuralBC(structuralmodel,"Edge",4,"RDisplacement",50e-6);
Fix axial displacement of a point on the hub to prevent rigid body motion.
structuralBC(structuralmodel,"Vertex",1,"ZDisplacement",0);
Generate a mesh.
generateMesh(structuralmodel);
Solve the model.
structuralresults = solve(structuralmodel);
Plot the radial displacement of the disk.
figure pdeplot(structuralmodel, ... "XYData",structuralresults.Displacement.ur, ... "ColorMap","jet") axis equal xlim([0 0.3]) ylim([-0.05 0.05])
Plot circumferential (hoop) stress.
figure pdeplot(structuralmodel, ... "XYData",structuralresults.Stress.sh, ... "ColorMap","jet") axis equal xlim([0 0.3]) ylim([-0.05 0.05])
Specify Nonconstant Displacement by Using Function Handle
Use a function handle to specify a harmonically varying excitation in a beam.
Create a transient dynamic model for a 3-D problem.
structuralmodel = createpde("structural","transient-solid");
Create a geometry and include it in the model. Plot the geometry.
gm = multicuboid(0.06,0.005,0.01); structuralmodel.Geometry = gm; pdegplot(structuralmodel,"FaceLabels","on","FaceAlpha",0.5) view(50,20)
Specify Young's modulus, Poisson's ratio, and the mass density of the material.
structuralProperties(structuralmodel,"YoungsModulus",210E9, ... "PoissonsRatio",0.3, ... "MassDensity",7800);
Fix one end of the beam.
structuralBC(structuralmodel,"Face",5,"Constraint","fixed");
Apply a sinusoidal displacement along the y-direction on the end opposite to the fixed end of the beam.
yDisplacementFunc = ... @(location,state) ones(size(location.y))*1E-4*sin(50*state.time); structuralBC(structuralmodel,"Face",3, ... "YDisplacement",yDisplacementFunc);
Apply Sinusoidal Displacement by Specifying Frequency
Specify a harmonically varying excitation by specifying its frequency.
Create a transient dynamic model for a 3-D problem.
structuralmodel = createpde("structural","transient-solid");
Create a geometry and include it in the model. Plot the geometry.
gm = multicuboid(0.06,0.005,0.01); structuralmodel.Geometry = gm; pdegplot(structuralmodel,"FaceLabels","on","FaceAlpha",0.5) view(50,20)
Specify Young's modulus, Poisson's ratio, and the mass density of the material.
structuralProperties(structuralmodel,"YoungsModulus",210E9, ... "PoissonsRatio",0.3, ... "MassDensity",7800);
Fix one end of the beam.
structuralBC(structuralmodel,"Face",5,"Constraint","fixed");
Apply a sinusoidal displacement along the y-direction on the end opposite to the fixed end of the beam.
structuralBC(structuralmodel,"Face",3, ... "YDisplacement",1E-4, ... "Frequency",50);
Specify Displacement at Corner of Rectangle
Fix one corner of a rectangular plate to restrain all rigid body motions of the model.
Create a structural model for static plane-stress analysis.
model = createpde("structural","static-planestress");
Create the geometry and include it in the structural model.
length = 1; width = 0.5; radius = 0.1; R1 = [3 4 -length length length -length ... -width -width width width]'; C1 = [1 0 0 radius 0 0 0 0 0 0]'; gdm = [R1 C1]; ns = char('R1','C1'); g = decsg(gdm,'R1- C1',ns'); geometryFromEdges(model,g);
Plot the geometry, displaying edge labels.
figure pdegplot(model,"EdgeLabels","on"); axis([-1.2*length 1.2*length ... -1.2*width 1.2*width])
Plot the geometry, displaying vertex labels.
figure pdegplot(model,"VertexLabels","on"); axis([-1.2*length 1.2*length ... -1.2*width 1.2*width])
Specify Young's modulus and Poisson's ratio of the material.
structuralProperties(model,"YoungsModulus",210E9,"PoissonsRatio",0.3);
Set the x-component of displacement on the left edge of the plate to zero to resist the applied load.
structuralBC(model,"Edge",3,"XDisplacement",0);
Apply the surface traction with a nonzero x-component on the right edge of the plate.
structuralBoundaryLoad(model,"Edge",1,"SurfaceTraction",[100000 0]);
Set the y-component of displacement at the bottom-left corner (vertex 3) to zero to restraint the rigid body motion.
structuralBC(model,"Vertex",3,"YDisplacement",0);
Generate the mesh, using Hmax to control the mesh size. A fine mesh lets you capture the gradation in the solution accurately.
generateMesh(model,"Hmax",radius/6);Solve the problem.
R = solve(model);
Plot the x-component of the normal stress distribution.
pdeplot(model,"XYData",R.Stress.sxx); axis equal colormap jet title("Normal Stress Along x-Direction")
Set Multipoint Constraint and Obtain ROM Results Compatible with Simscape Multibody™
Set multipoint constraints on two opposite sides of a beam.
Create a transient structural model for a 3-D problem.
structuralmodel = createpde("structural","transient-solid");
Create a geometry and include it in the model. Plot the geometry.
gm = multicuboid(0.1,0.01,0.01); structuralmodel.Geometry = gm; pdegplot(structuralmodel,"EdgeLabels","on","FaceAlpha",0.5)
Specify Young's modulus, Poisson's ratio, and the mass density of the material.
structuralProperties(structuralmodel,"YoungsModulus",70E9, ... "PoissonsRatio",0.3, ... "MassDensity",2700);
Generate a mesh.
generateMesh(structuralmodel);
Set the multipoint constraint on the right side of the beam. For better performance, set the constraint on the set of edges bounding the right side of the beam instead of setting it on the entire face.
structuralBC(structuralmodel,"Edge",[4,6,9,10], ... "Constraint","multipoint")
ans =
StructuralBC with properties:
RegionType: 'Edge'
RegionID: [4 6 9 10]
Vectorized: 'off'
Boundary Constraints and Enforced Displacements
Displacement: []
XDisplacement: []
YDisplacement: []
ZDisplacement: []
Constraint: "multipoint"
Radius: []
Reference: []
Label: []
Boundary Loads
Force: []
SurfaceTraction: []
Pressure: []
TranslationalStiffness: []
Label: []
Time Variation of Force, Pressure, or Enforced Displacement
StartTime: []
EndTime: []
RiseTime: []
FallTime: []
Sinusoidal Variation of Force, Pressure, or Enforced Displacement
Frequency: []
Phase: []
Using the same approach, set the multipoint constraint on the left side of the beam.
structuralBC(structuralmodel,"Edge",[2,8,11,12], ... "Constraint","multipoint")
ans =
StructuralBC with properties:
RegionType: 'Edge'
RegionID: [2 8 11 12]
Vectorized: 'off'
Boundary Constraints and Enforced Displacements
Displacement: []
XDisplacement: []
YDisplacement: []
ZDisplacement: []
Constraint: "multipoint"
Radius: []
Reference: []
Label: []
Boundary Loads
Force: []
SurfaceTraction: []
Pressure: []
TranslationalStiffness: []
Label: []
Time Variation of Force, Pressure, or Enforced Displacement
StartTime: []
EndTime: []
RiseTime: []
FallTime: []
Sinusoidal Variation of Force, Pressure, or Enforced Displacement
Frequency: []
Phase: []
Reduce the model to all modes in the frequency range [-Inf,500000] and the interface degrees of freedom.
R = reduce(structuralmodel,"FrequencyRange",[-Inf,500000]);Input Arguments
structuralmodel — Structural model
StructuralModel object
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","transient-solid")
RegionType — Geometric region type
"Vertex" | "Edge" | "Face" (for a 3-D model only)
Geometric region type, specified as "Vertex",
"Edge", or, for a 3-D model,
"Face".
You cannot use the following geometric region types if you specify the
"roller" or "symmetric" value for
the boundary constraint Cval:
"Edge"for a 3-D model"Vertex"for a 2-D or 3-D model
Example: structuralBC(structuralmodel,"Face",[2,5],"XDisplacement",0.1)
Data Types: char | string
RegionID — Geometric region ID
vector of positive integers
Geometric region ID, specified as a vector of positive integers. Find the
region IDs by using pdegplot.
Example: structuralBC(structuralmodel,"Face",[2,5],"XDisplacement",0.01)
Data Types: double
Dval — Enforced displacement
numeric vector | function handle
Enforced displacement, specified as a numeric vector or function handle. A
numeric vector must contain two elements for a 2-D model (including
axisymmetric models) and three elements for a 3-D model. The function must
return a two-row matrix for a 2-D model and a three-row matrix for a 3-D
model. Each column of the matrix must correspond to an enforced displacement
vector at the boundary coordinates provided by the solver. In case of a
transient or frequency response analysis, Dval also can
be a function of time or frequency, respectively. For details, see More About.
Note that when you specify Dval for an axisymmetric
model, the radial displacement on the axis of rotation must always be
zero.
Example: structuralBC(structuralmodel,"Face",[2,5],"Displacement",[0;0;0.01])
Data Types: double | function_handle
XDval — x-component of enforced displacement
number | function handle
x-component of enforced displacement, specified as a number or function
handle. The function must return a row vector. Each element of this vector
corresponds to the x-component value of the enforced displacement at the
boundary coordinates provided by the solver. In case of a transient or
frequency response analysis, XDval also can be a function
of time or frequency, respectively. For details, see More About.
Example: structuralBC(structuralmodel,"Face",[2,5],"XDisplacement",0.01)
Data Types: double | function_handle
YDval — y-component of enforced displacement
number | function handle
y-component of enforced displacement, specified as a number or function
handle. The function must return a row vector. Each element of this vector
corresponds to the y-component value of the enforced displacement at the
boundary coordinates provided by the solver. In case of a transient or
frequency response analysis, YDval also can be a function
of time or frequency, respectively. For details, see More About.
Example: structuralBC(structuralmodel,"Face",[2,5],"YDisplacement",0.01)
Data Types: double | function_handle
ZDval — z-component of enforced displacement
number | function handle
z-component of enforced displacement, specified as a number or function
handle. The function must return a row vector. Each element of this vector
corresponds to the z-component value of the enforced displacement at the
boundary coordinates provided by the solver. For a transient or frequency
response analysis, ZDval also can be a function of time
or frequency, respectively. For details, see More About.
You can specify ZDval for a 3-D or axisymmetric
model.
Example: structuralBC(structuralmodel,"Face",[2,5],"ZDisplacement",0.01)
Data Types: double | function_handle
RDval — r-component of enforced displacement
number | function handle
r-component of enforced displacement, specified as a number or function
handle. The function must return a row vector. Each element of this vector
corresponds to the r-component value of the enforced displacement at the
boundary coordinates provided by the solver. For a transient or frequency
response analysis, RDval also can be a function of time
or frequency, respectively. For details, see More About.
You can specify RDval only for an axisymmetric model.
RDval must be zero on the axis of rotation.
Example: structuralBC(structuralmodel,"Face",[2,5],"RDisplacement",0.01)
Data Types: double | function_handle
Cval — Standard structural boundary constraints
"free" (default) | "fixed" | "roller" | "symmetric" | "multipoint"
Standard structural boundary constraints, specified as
"free","fixed","roller",
"symmetric", or
"multipoint".
You cannot use the "roller" and
"symmetric" values with the following geometric
region types:
"Edge"for a 3-D model"Vertex"for a 2-D or 3-D model
Example: structuralBC(structuralmodel,"Face",[2,5],"Constraint","fixed")
Data Types: char | string
Coords — Reference point location for multipoint constraint
2-by-1 numeric vector | 3-by-1 numeric vector
Reference point location for the multipoint constraint, specified as a 2-by-1 (for a 2-D geometry) or 3-by-1 (for a 3-D geometry) numeric vector.
Example: structuralBC(structuralmodel,"Vertex",[1,3,5:10],"Constraint","multipoint","Reference",[0;0;1])
Data Types: double
R — Radius of circle (for 2-D geometry) or sphere (for 3-D geometry) around reference point location for multipoint constraint
positive number
Radius of a circle (for a 2-D geometry) or a sphere (for a 3-D geometry) around the reference point location for the multipoint constraint, specified as a positive number.
Example: structuralBC(structuralmodel,"Vertex",[1,3,5:10],"Constraint","multipoint","Reference",[0;0;1],"Radius",0.2)
Data Types: double
labeltext — Label for structural boundary condition
character vector | string
Label for the structural boundary condition, specified as a character vector or a string.
Data Types: char | string
Name-Value Arguments
Example: structuralBC(structuralmodel,"Face",[2,5],"XDisplacement",0.01,"RiseTime",0.5,"FallTime",0.5,"EndTime",3)
Use one or more name-value pair arguments to specify the form and duration of the
time-varying value of a component of displacement. Specify the displacement value
using one of the following arguments: XDval,
YDval, ZDval, or
RDval. You cannot use these name-value pair arguments to
specify more than one time-varying component or to specify the
Dval value.
You can model rectangular, triangular, and trapezoidal displacement pulses. If the start time is 0, you do not need to specify it.
For a rectangular pulse, specify the start and end times.
For a triangular pulse, specify the start time and any two of the following times: rise time, fall time, and end time. You also can specify all three times, but they must be consistent.
For a trapezoidal pulse, specify all four times.
You can model a harmonic displacement by specifying its frequency and initial phase. If the initial phase is 0, you do not need to specify it.
Output Arguments
More About
Tips
Restrain all rigid body motions by specifying as many boundary conditions as needed. If you do not restrain all rigid body motions, the entire geometry can freely rotate or move. The resulting linear system of equations is singular. The system can take a long time to converge, or it might not converge at all. If the system converges, the solution includes a large rigid body motion in addition to deformation.
Version History
Introduced in R2017b
You can also select a web site from the following list
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)
Asia Pacific
- Australia (English)
- India (English)
- New Zealand (English)
- 中国
- 日本Japanese (日本語)
- 한국Korean (한국어)