Stress Linearization


	The information about stress linearization is applicable if your license includes the Structural Mechanics Module.

Stress linearization is a procedure in which the stress distribution along a line through the thickness in a solid is approximated with an equivalent linear stress distribution, similar to what would be the result of an analysis using shell theory. The line is commonly referred to a stress classification line, SCL. This type of evaluation is common is the analysis of pressure vessels. It is also useful for the dimensioning of reinforcements for concrete structures, and for fatigue analysis of welds.

To perform a stress linearization, you add one Stress Linearization node for each SCL.

Orientation of Stress Components

The stresses along the SCL are represented in a local orthonormal coordinate system, x1-x2-x3. The x1 direction is oriented along the SCL, so it is mainly the stresses in the second and third directions which are of interest.

•

In 3D, you must specify the x2 direction, and thus implicitly the x3 direction. You specify the orientation either by selecting a point in the x1-x2 plane, or by defining an orientation vector in an approximate x2 direction. In either case, the actual x2 direction is chosen so that it is perpendicular to the SCL, and lies in the plane you have specified. The x3 orientation is then taken as perpendicular to x1 and x2. As long as you are only interested in a stress intensity, the choice of orientation is arbitrary.

•

In 2D, the x3 direction is the out-of-plane direction, and the x2 direction is perpendicular to the SCL in the X-Y plane.

•

In 2D axial symmetry, the x3 direction is the azimuthal direction, and the x2 direction is perpendicular to the SCL in the R-Z plane.

Creating the Stress Classification Line

The most straightforward way to create an SCL, is to include it in the geometry, and then select it in a node.

Figure 2-22: Four stress classification lines in a transition region at a pressure vessel nozzle.

There are, however, some situations where the direct approach is less convenient:

•

When the introduction of the SCL in the geometry must be done after the analysis, since the locations of critical regions were not obvious when setting up the initial analysis. It is of course possible to add new edges and rerun the analysis, but this may not be a good solutions if the analysis time is long.

•

When the introduction of the edges for the SCL makes the meshing more difficult. It may for example not any longer be possible to use swept meshes, or the mesh quality is reduced in critical regions.

In this case, a possible solution is to operate on a copy of the geometry in another component. It is then possible to use submodeling — that is, to study only a local region with its boundaries having displacements controlled by the solution from the larger model.

Below is an outline of the steps you need to take for this approach.

In the original component (assume that its tag is comp1), add a operator. Set to . You can name the operator, but in the following description, the default name genext1 is assumed. This operator will be used for mapping results to the second component.

Add a new component of the same dimension as the one in which you performed the original analysis.

Add the geometry, using for example or . to the new component (comp2).

Add the lines you are going to use for stress linearization to the imported geometry.

Add a Solid Mechanics interface, and select only the domains which contain the new lines. You can even change the geometry so that you cut out parts of the domains.

Add a node having domain selection. Select . Prescribe the displacement in all directions to be the same as in the original model with expressions like comp1.genext1(u) for .

If the original analysis contains inelastic strains, such as thermal expansions, these must also be included. You can do this either by adding a node with appropriate settings, or by explicitly importing the inelastic strains using an node. In the latter case, you would use expressions like comp1.genext1(solid.eth11) for the strain components.

Add nodes for the new linearization lines.

Add the materials that were used in comp1. The most efficient approach is to add them under and link to the same material definitions from both components.

Create a mesh for the domains in comp2 which you are solving for. It is only the mesh close to the new edges to which you need to pay any attention.

Add a new stationary study, in which you solve only for the new Solid Mechanics interface in comp2.

In the settings for the new study set to point to the solution from which you want to pick the results in comp1. You can also add an , if the original analysis contains results for several parameters or time steps.

Run the new study.

Studies and Solutions

Stress linearization is a pure postprocessing operation. The node will only create a number of variables, which can be evaluated under . It is thus possible to add such nodes after the main analysis has been performed. In order to make the new variables available for postprocessing, you must then run an .

Results

When you have included one or more nodes in a model, a number of data sets and an extra default plot are generated.

One edge data set is created for each SCL. These data sets are named Linearization Line <n>, where n is an integer number.

Figure 2-23: Generated data sets in a model with four SCL.

The default plot contains graphs for the 22 component of the actual stress, the membrane stress, and the linearized stress. The first Linearization Line data set is selected. By changing edge date set in the plot group, you can easily move between the different stress classification lines.

Figure 2-24: Default plot along a stress classification line.

Variable Names

Each node adds a number of variables. Many of these variables exist with two different scopes, physics scope and feature scope. The physics scope is the name of the physics interface, having the default value ‘solid’. The feature scope contains also the tag of the node, for example ‘sl1’.

As an example, the variable solid.Sm22 and the variable solid.sl1.Sm22 have the same value. The variables with physics scope makes it more convenient to create expressions using postprocessing. You could for example make a line plot of solid.sb22, and get all edges having a stress linearization colored by their individual results.

Table 2-13: Variable for stress linearization
Variable	Description	Variable in theory Section	Comment	Scope
Sllij	Stress tensor in local coordinate system		ij = 11, 12, 13, 22, 23, 33	Physics, Feature
Smij	Membrane stress		ij = 11, 12, 13, 22, 23, 33	Physics, Feature
Sbmaxij	Maximum bending stress		ij = 11, 12, 13, 22, 23, 33	Feature
Sbij	Bending Stress		ij = 11, 12, 13, 22, 23, 33	Physics, Feature
Smbij	Membrane + bending stress		ij = 11, 12, 13, 22, 23, 33	Physics, Feature
Spsij	Peak stress, starting point		ij = 11, 12, 13, 22, 23, 33	Feature
Speij	Peak stress, starting point		ij = 11, 12, 13, 22, 23, 33	Feature
SIm	Stress intensity, membrane			Physics, Feature
SImbs	Stress intensity, membrane + bending, starting point			Feature
SIbme	Stress intensity, membrane + bending, endpoint			Feature
SImb	Stress intensity, membrane + bending,		max(SImbs, SImbe)	Physics, Feature
Nij	Local in-plane force		ij = 22, 23, 33	Feature
Mij	Local bending moment		ij = 22, 23, 33	Feature
Qi	Local out-of-plane shear force		i = 2, 3	Feature
lengthtot	Length of SCL			Feature
arclength	Coordinate along SCL			Feature


	Stress Linearization in the Structural Mechanics Theory Chapter.