# structuralIC

Set initial conditions for a transient 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

`structuralIC(`

sets initial displacement and velocity for the entire geometry.`structuralmodel`

,"Displacement",`u0`

,"Velocity",`v0`

)

`structuralIC(___`

sets initial displacement and velocity for a particular geometry region using the
arguments from the previous syntax.`RegionType`

,`RegionID`

)

`structuralIC(`

sets initial displacement and velocity using the solution
`structuralmodel`

,`Sresults`

)`Sresults`

from a previous structural analysis on the same
geometry. If `Sresults`

is obtained by solving a transient
structural problem, then `structuralIC`

uses the solution
`Sresults`

for the last time-step.

`structuralIC(`

uses the solution `structuralmodel`

,`Sresults`

,`iT`

)`Sresults`

for the time-step
`iT`

from a previous structural analysis on the same
geometry.

returns a handle to the structural initial conditions object.`struct_ic`

= structuralIC(___)

## Examples

### Specify Initial Velocity

Specify initial velocity values for the entire geometry and for a particular face.

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

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

Create a geometry and include it into 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 the zero initial velocity on the entire geometry. When you specify only the initial velocity or initial displacement, `structuralIC`

assumes that the omitted parameter is zero. For example, here the initial displacement is also zero.

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

ans = GeometricStructuralICs with properties: RegionType: 'Cell' RegionID: 1 InitialDisplacement: [] InitialVelocity: [3x1 double]

Update the initial velocity on face 2 to model impulsive excitation.

structuralIC(structuralmodel,"Face",2,"Velocity",[0;60;0])

ans = GeometricStructuralICs with properties: RegionType: 'Face' RegionID: 2 InitialDisplacement: [] InitialVelocity: [3x1 double]

### Specify Nonconstant Initial Displacement by Using Function Handle

Specify initial *z*-displacement to be dependent on the coordinates *x* and *y*.

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

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

Create the geometry and include it into 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 the zero initial displacement on the entire geometry.

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

ans = GeometricStructuralICs with properties: RegionType: 'Cell' RegionID: 1 InitialDisplacement: [3x1 double] InitialVelocity: []

Now change the initial displacement in the *z*-direction on face 2 to a function of the coordinates *x* and *y*:

$$\mathit{u}\left(0\right)=\left[\begin{array}{c}0\\ 0\\ {\mathit{x}}^{2}+{\mathit{y}}^{2}\end{array}\right]$$

Write the following function file. Save it to a location on your MATLAB® path.

`function uinit = initdisp(location)`

` M = length(location.x);`

` uinit = zeros(3,M);`

` uinit(3,:) = location.x.^2 + location.y.^2;`

Pass the initial displacement to your structural model.

structuralIC(structuralmodel,"Face",2,"Displacement",@initdisp)

ans = GeometricStructuralICs with properties: RegionType: 'Face' RegionID: 2 InitialDisplacement: @initdisp InitialVelocity: []

### Use Static Solution as Initial Condition

Use a static solution as an initial condition for a dynamic structural model.

Create a static model.

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

Create the geometry and include it in the model. Plot the geometry.

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

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

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

Apply the boundary condition and static load.

structuralBC(staticmodel,"Face",5,"Constraint","fixed"); structuralBoundaryLoad(staticmodel,"Face",3, ... "SurfaceTraction", ... [0;1E6;0]);

Generate a mesh and solve the model.

```
generateMesh(staticmodel,"Hmax",0.02);
Rstatic = solve(staticmodel);
```

Create a dynamic model and assign geometry.

dynamicmodel = createpde("structural","transient-solid"); gm = multicuboid(0.06,0.005,0.01); dynamicmodel.Geometry = gm;

Apply the boundary condition.

structuralBC(dynamicmodel,"Face",5,"Constraint","fixed");

Generate a mesh.

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

Specify the initial condition using the static solution.

structuralIC(dynamicmodel,Rstatic)

ans = NodalStructuralICs with properties: InitialDisplacement: [189x3 double] InitialVelocity: [189x3 double]

## Input Arguments

`structuralmodel`

— Transient structural model

`StructuralModel`

object

Transient structural model, specified as a
`StructuralModel`

object. The model contains the
geometry, mesh, structural properties of the material, body loads, boundary
loads, boundary conditions, and initial conditions.

**Example: **```
structuralmodel =
createpde("structural","transient-solid")
```

`u0`

— Initial displacement

numeric vector | function handle

Initial displacement, 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 elements represent the components of initial displacement.

Use a function handle to specify spatially varying initial displacement. 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 corresponds to the initial displacement at the coordinates provided by the solver. For details, see More About.

**Example: **`structuralIC(structuralmodel,"Face",[2,5],"Displacement",[0;0;0.01])`

**Data Types: **`double`

| `function_handle`

`v0`

— Initial velocity

numeric vector | function handle

Initial velocity, 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 elements represent the components of initial velocity.

Use a function handle to specify spatially varying initial velocity. 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 corresponds to the initial velocity at the coordinates provided by the solver. For details, see More About.

**Example: **`structuralIC(structuralmodel,"Face",[2,5],"Displacement",[0;0;0.01],"Velocity",[0;60;0])`

**Data Types: **`double`

| `function_handle`

`RegionType`

— Geometric region type

`"Face"`

| `"Edge"`

| `"Vertex"`

| `"Cell"`

Geometric region type, specified as `"Face"`

,
`"Edge"`

, `"Vertex"`

, or
`"Cell"`

.

When you apply multiple initial condition assignments, the solver uses these precedence rules for determining the initial condition.

For multiple assignments to the same geometric region, the solver uses the last applied setting.

For separate assignments to a geometric region and the boundaries of that region, the solver uses the specified assignment on the region and chooses the assignment on the boundary as follows. The solver gives an

`"Edge"`

assignment precedence over a`"Face"`

assignment, even if you specify a`"Face"`

assignment after an`"Edge"`

assignment. The precedence levels are`"Vertex"`

(highest precedence),`"Edge"`

,`"Face"`

,`"Cell"`

(lowest precedence).For an assignment made with the

`results`

object, the solver uses that assignment instead of all previous assignments.

**Example: **`structuralIC(structuralmodel,"Face",[2,5],"Displacement",[0;0;0.01],"Velocity",[0;60;0])`

**Data Types: **`char`

`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: **`structuralIC(structuralmodel,"Face",[2,5],"Displacement",[0;0;0.01],"Velocity",[0;60;0])`

**Data Types: **`double`

`Sresults`

— Structural model solution

`StaticStructuralResults`

object | `TransientStructuralResults`

object

Structural model solution, specified as a
`StaticStructuralResults`

or
`TransientStructuralResults`

object. Create
`Sresults`

by using `solve`

.

`iT`

— Time index

positive integer

Time index, specified as a positive integer.

**Example: **`structuralIC(structuralmodel,Sresults,21)`

**Data Types: **`double`

## Output Arguments

`struct_ic`

— Handle to initial conditions

`GeometricStructuralICs`

object | `NodalStructuralICs`

object

Handle to initial conditions, returned as a
`GeometricStructuralICs`

or
`NodalStructuralICs`

object. See GeometricStructuralICs Properties and NodalStructuralICs Properties.

`structuralIC`

associates the structural initial
condition with the geometric region in the case of a geometric assignment,
or the nodes in the case of a results-based assignment.

## 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 R2018a**

## Comando de MATLAB

Ha hecho clic en un enlace que corresponde a este comando de MATLAB:

Ejecute el comando introduciéndolo en la ventana de comandos de MATLAB. Los navegadores web no admiten comandos de MATLAB.

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)