# structuralBoundaryLoad

Specify boundary loads 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

`structuralBoundaryLoad(`

specifies the surface traction, pressure, and translational stiffness on the
boundary of type `structuralmodel`

,`RegionType`

,`RegionID`

,"SurfaceTraction",`STval`

,"Pressure",`Pval`

,"TranslationalStiffness",`TSval`

)`RegionType`

with
`RegionID`

ID numbers.

Surface traction is determined as distributed normal and tangential forces acting on a boundary, resolved along the global Cartesian coordinate system.

Pressure must be specified in the direction that is normal to the boundary. A positive pressure value acts into the boundary (for example, compression). A negative pressure value acts away from the boundary (for example, suction).

Translational stiffness is a distributed spring stiffness for each translational direction. Translational stiffness is used to model an elastic foundation.

`structuralBoundaryLoad`

does not require you to specify
all three boundary loads. Depending on your structural analysis problem, you can
specify one or more boundary loads by picking the corresponding arguments and
omitting others. You can specify translational stiffness for any structural
model. To specify pressure or surface traction,
`structuralmodel`

must be a static, transient, or
frequency response model. Structural models for modal analysis cannot have
pressure or surface traction.

The default boundary load is a stress-free boundary condition.

`structuralBoundaryLoad(`

specifies concentrated force at a vertex with the `structuralmodel`

,"Vertex",`VertexID`

,"Force",`Fval`

)`VertexID`

number. You can specify force only if `structuralmodel`

is a
static, transient, or frequency response model. Structural models for modal
analysis cannot have concentrated force.

`structuralBoundaryLoad(___,"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.

`structuralBoundaryLoad(___,"Pressure",`

lets you specify the form and duration of a nonconstant pressure pulse and
harmonic excitation for a transient structural model without creating a function
handle. When using this syntax, you must specify the model, region type and
region ID, and pressure. Surface traction and translational stiffness are
optional arguments. This syntax does not work for static, modal analysis, and
frequency response models.`Pval`

,`Name,Value`

)

`structuralBoundaryLoad(`

lets you specify the form and duration of a nonconstant concentrated force and
harmonic excitation for a transient structural model without creating a function
handle.`structuralmodel`

,"Vertex",`VertexID`

,"Force",`Fval`

,`Name,Value`

)

`structuralBoundaryLoad(___,"Label",`

adds a label for the structural boundary load to be used by the `labeltext`

)`linearizeInput`

function. This function lets you pass boundary
loads to the `linearize`

function that extracts sparse linear models for use
with Control System Toolbox™.

returns the boundary load object.`boundaryLoad`

= structuralBoundaryLoad(___)

## 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 Translational Stiffness

Create a structural model.

structuralModel = createpde("structural","static-solid");

Create a block geometry.

gm = multicuboid(20,10,5);

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 and Poisson's ratio.

structuralProperties(structuralModel,"YoungsModulus",30, ... "PoissonsRatio",0.3);

The bottom face of the block rests on an elastic foundation (a spring). To model this foundation, specify the translational stiffness.

structuralBoundaryLoad(structuralModel, ... "Face",1, ... "TranslationalStiffness",[0;0;30])

ans = StructuralBC with properties: RegionType: 'Face' RegionID: 1 Vectorized: 'off' Boundary Constraints and Enforced Displacements Displacement: [] XDisplacement: [] YDisplacement: [] ZDisplacement: [] Constraint: [] Radius: [] Reference: [] Label: [] Boundary Loads Force: [] SurfaceTraction: [] Pressure: [] TranslationalStiffness: [3x1 double] Label: []

### Apply Concentrated Force at Point

Specify a force value at a vertex of a geometry.

Create a structural model for static analysis of a solid (3-D) problem.

model = createpde("structural","static-solid");

Create the geometry, which consists of two cuboids stacked on top of each other.

`gm = multicuboid(0.2,0.01,[0.01 0.01],"Zoffset",[0 0.01]);`

Include the geometry in the structural model.

model.Geometry = gm;

Plot the geometry and display the face labels. Rotate the geometry so that you can see the face labels on the left side.

figure pdegplot(model,"FaceLabels","on"); view([-67 5])

Plot the geometry and display the vertex labels. Rotate the geometry so that you can see the vertex labels on the right side.

figure pdegplot(model,"VertexLabels","on","FaceAlpha",0.5) xlim([-0.01 0.1]) zlim([-0.01 0.02]) view([60 5])

Specify Young's modulus, Poisson's ratio, and the mass density of the material.

structuralProperties(model,"YoungsModulus",201E9,"PoissonsRatio",0.3);

Specify that faces 5 and 10 are fixed boundaries.

structuralBC(model,"Face",[5 10],"Constraint","fixed");

Specify the concentrated force at vertex 6.

structuralBoundaryLoad(model,"Vertex",6,"Force",[0;10^4;0])

ans = StructuralBC with properties: RegionType: 'Vertex' RegionID: 6 Vectorized: 'off' Boundary Constraints and Enforced Displacements Displacement: [] XDisplacement: [] YDisplacement: [] ZDisplacement: [] Constraint: [] Radius: [] Reference: [] Label: [] Boundary Loads Force: [3x1 double] SurfaceTraction: [] Pressure: [] TranslationalStiffness: [] Label: []

### Specify Pressure for Frequency Response Model

Use a function handle to specify a frequency-dependent pressure for a frequency response model.

Create a frequency response model for a 3-D problem.

fmodel = createpde("structural","frequency-solid");

Import and plot the geometry.

importGeometry(fmodel,"TuningFork.stl"); figure pdegplot(fmodel,"FaceLabels","on")

Specify the pressure loading on a tine (face 11) as a short rectangular pressure pulse. In the frequency domain, this pressure pulse is a unit load uniformly distributed across all frequencies.

structuralBoundaryLoad(fmodel,"Face",11,"Pressure",1);

Now specify a frequency-dependent pressure load, for example, $\mathit{p}={\mathit{e}}^{-{\left(\omega -1000\right)}^{2}/100000}$.

pLoad = @(location,state) exp(-(state.frequency-1E3).^2/1E5); structuralBoundaryLoad(fmodel,"Face",12,"Pressure",pLoad);

### Specify Nonconstant Pressure For Transient Model by Using Function Handle

Use a function handle to specify a harmonically varying pressure at the center of a thin 3-D plate.

Create a transient dynamic model for a 3-D problem.

structuralmodel = createpde("structural","transient-solid");

Create a geometry consisting of a thin 3-D plate with a small plate at the center. Include the geometry in the model and plot it.

gm = multicuboid([5,0.05],[5,0.05],0.01); structuralmodel.Geometry = gm; pdegplot(structuralmodel,"FaceLabels","on","FaceAlpha",0.5)

Zoom in to see the face labels on the small plate at the center.

figure pdegplot(structuralmodel,"FaceLabels","on","FaceAlpha",0.25) axis([-0.2 0.2 -0.2 0.2 -0.1 0.1])

Specify Young's modulus, Poisson's ratio, and the mass density of the material.

structuralProperties(structuralmodel,"YoungsModulus",210E9,... "PoissonsRatio",0.3,... "MassDensity",7800);

Specify that all faces on the periphery of the thin 3-D plate are fixed boundaries.

structuralBC(structuralmodel,"Constraint","fixed","Face",5:8);

Apply a harmonically varying pressure load on the small face at the center of the plate.

plungerLoad = @(location,state)5E7.*sin(25.*state.time); structuralBoundaryLoad(structuralmodel,"Face",12,"Pressure",plungerLoad)

ans = StructuralBC with properties: RegionType: 'Face' RegionID: 12 Vectorized: 'off' Boundary Constraints and Enforced Displacements Displacement: [] XDisplacement: [] YDisplacement: [] ZDisplacement: [] Constraint: [] Radius: [] Reference: [] Label: [] Boundary Loads Force: [] SurfaceTraction: [] Pressure: @(location,state)5E7.*sin(25.*state.time) TranslationalStiffness: [] Label: [] Time Variation of Force, Pressure, or Enforced Displacement StartTime: [] EndTime: [] RiseTime: [] FallTime: [] Sinusoidal Variation of Force, Pressure, or Enforced Displacement Frequency: [] Phase: []

### Apply Sinusoidal Pressure by Specifying Frequency

Specify a harmonically varying pressure at the center of a thin 3-D plate by specifying its frequency.

Create a transient dynamic model for a 3-D problem.

structuralmodel = createpde("structural","transient-solid");

Create a geometry consisting of a thin 3-D plate with a small plate at the center. Include the geometry in the model and plot it.

gm = multicuboid([5,0.05],[5,0.05],0.01); structuralmodel.Geometry=gm; pdegplot(structuralmodel,"FaceLabels","on","FaceAlpha",0.5)

Zoom in to see the face labels on the small plate at the center.

figure pdegplot(structuralmodel,"FaceLabels","on","FaceAlpha",0.25) axis([-0.2 0.2 -0.2 0.2 -0.1 0.1])

Specify Young's modulus, Poisson's ratio, and the mass density of the material.

structuralProperties(structuralmodel,"YoungsModulus",210E9,... "PoissonsRatio",0.3,... "MassDensity",7800);

Specify that all faces on the periphery of the thin 3-D plate are fixed boundaries.

structuralBC(structuralmodel,"Constraint","fixed","Face",5:8);

Apply a harmonically varying pressure load on the small face at the center of the plate.

structuralBoundaryLoad(structuralmodel,"Face",12, ... "Pressure",5E7, ... "Frequency",25)

ans = StructuralBC with properties: RegionType: 'Face' RegionID: 12 Vectorized: 'off' Boundary Constraints and Enforced Displacements Displacement: [] XDisplacement: [] YDisplacement: [] ZDisplacement: [] Constraint: [] Radius: [] Reference: [] Label: [] Boundary Loads Force: [] SurfaceTraction: [] Pressure: 50000000 TranslationalStiffness: [] Label: [] Time Variation of Force, Pressure, or Enforced Displacement StartTime: [] EndTime: [] RiseTime: [] FallTime: [] Sinusoidal Variation of Force, Pressure, or Enforced Displacement Frequency: 25 Phase: []

### Apply Rectangular Pressure Pulse on Boundary

Create a transient structural model.

structuralModel = createpde("structural","transient-solid");

Import and plot the geometry.

importGeometry(structuralModel,"BracketWithHole.stl"); pdegplot(structuralModel,"FaceLabels","on") view(-20,10)

Specify Young's modulus and Poisson's ratio.

structuralProperties(structuralModel,"YoungsModulus",200e9, ... "PoissonsRatio",0.3,... "MassDensity",7800);

Specify that face 4 is a fixed boundary.

structuralBC(structuralModel,"Face",4,"Constraint","fixed");

Apply a rectangular pressure pulse on face 7 in the direction normal to the face.

structuralBoundaryLoad(structuralModel,"Face",7,"Pressure",10^5,... "StartTime",0.1,"EndTime",0.5)

ans = StructuralBC with properties: RegionType: 'Face' RegionID: 7 Vectorized: 'off' Boundary Constraints and Enforced Displacements Displacement: [] XDisplacement: [] YDisplacement: [] ZDisplacement: [] Constraint: [] Radius: [] Reference: [] Label: [] Boundary Loads Force: [] SurfaceTraction: [] Pressure: 100000 TranslationalStiffness: [] Label: [] Time Variation of Force, Pressure, or Enforced Displacement StartTime: 0.1000 EndTime: 0.5000 RiseTime: [] FallTime: [] Sinusoidal Variation of Force, Pressure, or Enforced Displacement Frequency: [] Phase: []

### Apply Rectangular Force Pulse at Point

Specify a short concentrated force pulse at a vertex of a geometry.

Create a structural model for static analysis of a solid (3-D) problem.

structuralmodel = createpde("structural","transient-solid");

Create the geometry, which consists of two cuboids stacked on top of each other.

`gm = multicuboid(0.2,0.01,[0.01 0.01],"Zoffset",[0 0.01]);`

Include the geometry in the structural model.

structuralmodel.Geometry = gm;

Plot the geometry and display the face labels. Rotate the geometry so that you can see the face labels on the left side.

figure pdegplot(structuralmodel,"FaceLabels","on"); view([-67 5])

Plot the geometry and display the vertex labels. Rotate the geometry so that you can see the vertex labels on the right side.

figure pdegplot(structuralmodel,"VertexLabels","on","FaceAlpha",0.5) xlim([-0.01 0.1]) zlim([-0.01 0.02]) view([60 5])

Specify Young's modulus, Poisson's ratio, and the mass density of the material.

structuralProperties(structuralmodel,"YoungsModulus",201E9, ... "PoissonsRatio",0.3, ... "MassDensity",7800);

Specify that faces 5 and 10 are fixed boundaries.

structuralBC(structuralmodel,"Face",[5 10],"Constraint","fixed");

Specify a short concentrated force pulse at vertex 6.

structuralBoundaryLoad(structuralmodel,"Vertex",6, ... "Force",[0;1000;0], ... "StartTime",1, ... "EndTime",1.05)

ans = StructuralBC with properties: RegionType: 'Vertex' RegionID: 6 Vectorized: 'off' Boundary Constraints and Enforced Displacements Displacement: [] XDisplacement: [] YDisplacement: [] ZDisplacement: [] Constraint: [] Radius: [] Reference: [] Label: [] Boundary Loads Force: [3×1 double] SurfaceTraction: [] Pressure: [] TranslationalStiffness: [] Label: [] Time Variation of Force, Pressure, or Enforced Displacement StartTime: 1 EndTime: 1.0500 RiseTime: [] FallTime: [] Sinusoidal Variation of Force, Pressure, or Enforced Displacement Frequency: [] Phase: []

Specify zero initial displacement and velocity.

structuralIC(structuralmodel,"Displacement",[0;0;0],"Velocity",[0;0;0])

ans = GeometricStructuralICs with properties: RegionType: 'Cell' RegionID: [1 2] InitialDisplacement: [3×1 double] InitialVelocity: [3×1 double]

Generate a fine mesh.

`generateMesh(structuralmodel,"Hmax",0.02);`

Because the load is zero for the initial time span and is applied for only a short time, solve the model for two time spans. Use the first time span to find the solution before the force pulse.

structuralresults1 = solve(structuralmodel,0:1E-2:1);

Use the second time span to find the solution during and after the force pulse.

structuralIC(structuralmodel,structuralresults1)

ans = NodalStructuralICs with properties: InitialDisplacement: [1543×3 double] InitialVelocity: [1543×3 double]

```
structuralresults2 = solve(structuralmodel, ...
[1.001:0.001:1.01 1.02:1E-2:2]);
```

Plot the displacement value at the node corresponding to vertex 6, where you applied the concentrated force pulse.

loadedNd = findNodes(structuralmodel.Mesh,"region","Vertex",6); plot(structuralresults2.SolutionTimes, ... structuralresults2.Displacement.uy(loadedNd,:))

## 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

`"Edge"`

for a 2-D model | `"Face"`

for a 3-D model

Geometric region type, specified as `"Edge"`

for a 2-D
model or `"Face"`

for a 3-D model.

**Example: **`structuralBoundaryLoad(structuralmodel,"Face",[2,5],"SurfaceTraction",[0,0,100])`

**Data Types: **`char`

| `string`

`RegionID`

— Geometric region ID

positive integer | vector of positive integers

Geometric region ID, specified as a positive integer or vector of positive
integers. Find the region IDs by using `pdegplot`

.

**Example: **`structuralBoundaryLoad(structuralmodel,"Face",[2,5],"SurfaceTraction",[0,0,100])`

**Data Types: **`double`

`VertexID`

— Vertex ID

positive integer | vector of positive integers

Vertex ID, specified as a positive integer or vector of positive integers.
Find the vertex IDs using `pdegplot`

.

**Example: **`structuralBoundaryLoad(structuralmodel,"Vertex",6,"Force",[0;10^4;0])`

**Data Types: **`double`

`STval`

— Distributed normal and tangential forces on boundary

numeric vector | function handle

Distributed normal and tangential forces on the boundary, resolved along the global Cartesian coordinate system, specified as a numeric vector or function handle. A numeric vector must contain two elements for a 2-D model 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 the
surface traction vector at the boundary coordinates provided by the solver.
In case of a transient or frequency response analysis,
`STval`

also can be a function of time or frequency,
respectively. For details, see More About.

**Example: **`structuralBoundaryLoad(structuralmodel,"Face",[2,5],"SurfaceTraction",[0;0;100])`

**Data Types: **`double`

| `function_handle`

`Pval`

— Pressure normal to boundary

number | function handle

Pressure normal to the boundary, specified as a number or function handle. A positive-value pressure acts into the boundary (for example, compression), while a negative-value pressure acts away from the boundary (for example, suction).

If you specify `Pval`

as a function handle, the function
must return a row vector where each column corresponds to the value of
pressure at the boundary coordinates provided by the solver. In case of a
transient structural model, `Pval`

also can be a function
of time. In case of a frequency response structural model,
`Pval`

can be a function of frequency (when specified
as a function handle) or a constant pressure with the same magnitude for a
broad frequency spectrum. For details, see More About.

**Example: **`structuralBoundaryLoad(structuralmodel,"Face",[2,5],"Pressure",10^5)`

**Data Types: **`double`

| `function_handle`

`TSval`

— Distributed spring stiffness

numeric vector | function handle

Distributed spring stiffness for each translational direction used to
model elastic foundation, specified as a numeric vector or function handle.
A numeric vector must contain two elements for a 2-D model and three
elements for a 3-D model. The custom 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 this
matrix corresponds to the stiffness vector at the boundary coordinates
provided by the solver. In case of a transient or frequency response
analysis, `TSval`

also can be a function of time or
frequency, respectively. For details, see More About.

**Example: **`structuralBoundaryLoad(structuralmodel,"Edge",[2,5],"TranslationalStiffness",[0;5500])`

**Data Types: **`double`

| `function_handle`

`Fval`

— Concentrated force

numeric vector | function handle

Concentrated force at a vertex, specified as a numeric vector or function handle. Use a function handle to specify concentrated force that depends time or frequency. For details, see More About.

**Example: **`structuralBoundaryLoad(structuralmodel,"Vertex",5,"Force",[0;0;10])`

**Data Types: **`double`

| `function_handle`

`labeltext`

— Label for structural boundary load

character vector | string

Label for the structural boundary load, specified as a character vector or a string.

**Data Types: **`char`

| `string`

### Name-Value Arguments

**Example: **`structuralBoundaryLoad(structuralmodel,"Face",[2,5],"Pressure",10^5,"RiseTime",0.5,"FallTime",0.5,"EndTime",3)`

Use one or more of the name-value pair arguments to specify the form and duration
of the pressure or concentrated force pulse and harmonic excitation **for a transient structural model only**. Specify the
pressure or force value using the `Pval`

or
`Fval`

argument, respectively.

You can model rectangular, triangular, and trapezoidal pressure or concentrated force pulses. If the start time is 0, you can omit specifying 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 pressure or concentrated force load by specifying its frequency and initial phase. If the initial phase is 0, you can omit specifying it.

**Rectangular, Triangular, or Trapezoidal Pulse**

`StartTime`

— Start time for pressure or concentrated force load

nonnegative number

Start time for pressure or concentrated force load, specified as a nonnegative number. Specify this argument only for transient structural models.

**Example: **`structuralBoundaryLoad(structuralmodel,"Face",[2,5],"Pressure",10^5,"StartTime",1,"EndTime",3)`

**Data Types: **`double`

`EndTime`

— End time for pressure or concentrated force load

nonnegative number

End time for pressure or concentrated force load, specified as a nonnegative number equal or greater than the start time value. Specify this argument only for transient structural models.

**Example: **`structuralBoundaryLoad(structuralmodel,"Face",[2,5],"Pressure",10^5,"StartTime",1,"EndTime",3)`

**Data Types: **`double`

`RiseTime`

— Rise time for pressure or concentrated force load

nonnegative number

Rise time for pressure or concentrated force load, specified as a nonnegative number. Specify this argument only for transient structural models.

**Example: **`structuralBoundaryLoad(structuralmodel,"Face",[2,5],"Pressure",10^5,"RiseTime",0.5,"FallTime",0.5,"EndTime",3)`

**Data Types: **`double`

`FallTime`

— Fall time for pressure or concentrated force load

nonnegative number

Fall time for pressure or concentrated force load, specified as a nonnegative number. Specify this argument only for transient structural models.

**Example: **`structuralBoundaryLoad(structuralmodel,"Face",[2,5],"Pressure",10^5,"RiseTime",0.5,"FallTime",0.5,"EndTime",3)`

**Data Types: **`double`

**Harmonic Pressure or Force**

`Frequency`

— Frequency of sinusoidal pressure or concentrated force

positive number

Frequency of sinusoidal pressure or concentrated force, specified as a positive number, in radians per unit of time. Specify this argument only for transient structural models.

**Example: **`structuralBoundaryLoad(structuralmodel,"Face",[2,5],"Pressure",10^5,"Frequency",25)`

**Data Types: **`double`

`Phase`

— Phase of sinusoidal pressure or concentrated force

nonnegative number

Phase of sinusoidal pressure or concentrated force, specified as a nonnegative number, in radians. Specify this argument only for transient structural models.

**Example: **`structuralBoundaryLoad(structuralmodel,"Face",[2,5],"Pressure",10^5,"Frequency",25,"Phase",pi/6)`

**Data Types: **`double`

## Output Arguments

`boundaryLoad`

— Handle to boundary load

`StructuralBC`

object

Handle to boundary load, returned as a `StructuralBC`

object. See StructuralBC Properties.

## More About

### Specifying Nonconstant Parameters of a Structural Model

Use a function handle to specify the following structural parameters when they depend on space and, depending of the type of structural analysis, either time or frequency:

Surface traction on the boundary

Pressure normal to the boundary

Concentrated force at a vertex

Distributed spring stiffness for each translational direction used to model elastic foundation

Enforced displacement and its components

Initial displacement and velocity (can depend on space only)

For example, use function handles to specify the pressure load,
*x*-component of the enforced displacement, and the initial displacement
for this model.

structuralBoundaryLoad(model,"Face",12, ... "Pressure",@myfunPressure) structuralBC(model,"Face",2, ... "XDisplacement",@myfunBC) structuralIC(model,"Face",12, ... "Displacement",@myfunIC)

For all parameters, except the initial displacement and velocity, the function must be of the form:

`function structuralVal = myfun(location,state)`

For the initial displacement and velocity the function must be of the form:

`function structuralVal = myfun(location)`

The solver computes and populates the data in the `location`

and
`state`

structure arrays and passes this data to your function. You can
define your function so that its output depends on this data. You can use any names instead
of `location`

and `state`

, but the function must have
exactly two arguments (or one argument if the function specifies the initial displacement or
initial velocity).

`location`

— A structure containing these fields:`location.x`

— The*x*-coordinate of the point or points`location.y`

— The*y*-coordinate of the point or points`location.z`

— For a 3-D or an axisymmetric geometry, the*z*-coordinate of the point or points`location.r`

— For an axisymmetric geometry, the*r*-coordinate of the point or points

Furthermore, for boundary conditions, the solver passes these data in the

`location`

structure:`location.nx`

—*x*-component of the normal vector at the evaluation point or points`location.ny`

—*y*-component of the normal vector at the evaluation point or points`location.nz`

— For a 3-D or an axisymmetric geometry,*z*-component of the normal vector at the evaluation point or points`location.nr`

— For an axisymmetric geometry,*r*-component of the normal vector at the evaluation point or points

`state`

— A structure containing these fields for dynamic structural problems:`state.time`

contains the time at evaluation points.`state.frequency`

contains the frequency at evaluation points.

`state.time`

and`state.frequency`

are scalars.

Boundary constraints and loads get these data from the solver:

`location.x`

,`location.y`

,`location.z`

,`location.r`

`location.nx`

,`location.ny`

,`location.nz`

,`location.nr`

`state.time`

or`state.frequency`

(depending of the type of structural analysis)

Initial conditions get these data from the solver:

`location.x`

,`location.y`

,`location.z`

,`location.r`

Subdomain ID

If a parameter represents a vector value, such as surface traction, spring stiffness, force, or displacement, your 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 corresponds to the parameter value (a vector) at the boundary coordinates provided by the solver.

If a parameter represents a scalar value, such as pressure or a displacement component, your function must return a row vector where each element corresponds to the parameter value (a scalar) at the boundary coordinates provided by the solver.

If boundary conditions depend on `state.time`

or
`state.frequency`

, ensure that your function returns a matrix of
`NaN`

of the correct size when `state.frequency`

or
`state.time`

are `NaN`

. Solvers check whether a
problem is nonlinear or time dependent by passing `NaN`

state values and
looking for returned `NaN`

values.

### Additional Arguments in Functions for Nonconstant Structural Parameters

To use additional arguments in your function, wrap your function (that takes additional arguments) with an anonymous function that takes only the `location`

and `state`

arguments. For example:

structuralVal = ... @(location,state) myfunWithAdditionalArgs(location,state,arg1,arg2...) structuralBC(model,"Face",2,"XDisplacement",structuralVal) structuralVal = ... @(location) myfunWithAdditionalArgs(location,arg1,arg2...) structuralIC(model,"Face",2,"Displacement",structuralVal)

## Version History

**Introduced in R2017b**

### R2021b: Label to extract sparse linear models for use with Control System Toolbox

Now you can add a label for structural boundary loads to be used by the `linearizeInput`

function. This function lets you pass structural
boundary loads to the `linearize`

function that extracts sparse linear models for use with Control System Toolbox.

### R2019b: Concentrated boundary loads at arbitrary locations on geometry surfaces

You can now use `addVertex`

to create new vertices at any points on boundaries of a 2-D or 3-D geometry
represented by a `DiscreteGeometry`

object. Then set concentrated
boundary loads at these vertices.

### R2019a: Concentrated force at a vertex

You can now specify concentrated force at a vertex.

### R2018a: Time-dependent boundary loads

You can now specify time-dependent boundary loads by using function handles or specify the form and duration of the pressure pulse and the frequency and phase of sinusoidal pressure.

## 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)