#### 2.4 Plane Stress Elements

##### 2.4.1 PlaneStress2d

Represents isoparametric four-node quadrilateral plane-stress finite element. Each node has 2 degrees of freedom. Structure should be defined in x,y plane. The nodes should be numbered anti-clockwise (positive rotation around z-axis). The element features are summarized in Table 7.

The generalization of this element, that can be positioned arbitrarily in space is linquad3dplanestress element. This element requires 3 displacement degrees of freedon in each node and assumes, that the element geometry is flat, i.e. all nodes are in the same plane. The element features are summarized in Table 8.

 Keyword planestress2d Description 2D quadrilateral element for plane stress analysis Specific parameters [NIP #(in)] Parameters NIP: allows to set the number of integration points Unknowns Two dofs (u-displacement, v-displacement) are required in each node. Approximation Linear approximation of displacements and geometry. Integration Integration of membrane strain terms using Gauss integration formula in 1, 4 (default), 9 or 16 integration points. The default number of integration points used can be overloaded using NIP parameter. Reduced integration for shear terms is employed. Shear terms are always integrated using the 1-point integration rule. Features Nonlocal constitutive support, Geometric nonlinearity support. CS properties cross section thickness is required. Loads Body loads are supported. Boundary loads are supported and computed using numerical integration. The side numbering is following. Each i-th element side begins in i-th element node and ends on next element node (i+1-th node or 1-st node, in the case of side number 4). The local positive edge x-axis coincides with side direction, the positive local edge y-axis is rotated 90 degrees anti-clockwise (see fig. (5)). Nlgeo 0, 1. Status Reliable

Table 7: planestress2d element summary

 Keyword linquad3dplanestress Description 3D quadrilateral element for plane stress analysis Specific parameters [NIP #(in)] Parameters NIP: allows to set the number of integration points Unknowns Three dofs (u-displacement, v-displacement, w-displacement) are required in each node. Approximation Linear approximation of displacements and geometry. Integration Integration of membrane strain terms using Gauss integration formula in 1, 4 (default), 9 or 16 integration points. The default number of integration points used can be overloaded using NIP parameter. Reduced integration for shear terms is employed. Shear terms are always integrated using the 1-point integration rule. Features Nonlocal constitutive support, Geometric nonlinearity support. CS properties cross section thickness is required. Loads Body loads are supported. Boundary loads are supported and computed using numerical integration. The side numbering is following. Each i-th element side begins in i-th element node and ends on next element node (i+1-th node or 1-st node, in the case of side number 4). The local positive edge x-axis coincides with side direction, the positive local edge y-axis is rotated 90 degrees anti-clockwise (see fig. (5)). Nlgeo 0, 1. Status Basic functionality tested, element loads need further testing.

##### 2.4.2 QPlaneStress2d

Implementation of quadratic isoparametric eight-node quadrilateral plane-stress finite element. Each node has 2 degrees of freedom. The node numbering is anti-clockwise and is explained in fig. (6). The element features are summarized in Table 9.

 Keyword qplanestress2d Description 2D quadratic isoparametric plane stress element Specific parameters [NIP #(in)] Parameters NIP: allows to set the number of integration points Unknowns Two dofs (u-displacement, v-displacement) are required in each node. Approximation Quadratic approximation of displacements and geometry. Integration Full integration using Gauss integration formula in 4 (the default), 9 or 16 integration points. The default number of integration points used can be overloaded using NIP parameter. Features Adaptivity support. CS properties Cross section thickness is required. Loads Body and boundary loads are supported. Nlgeo 0, 1. Status Stable

Table 9: qplanestress2d element summary

##### 2.4.3 TrPlaneStress2d

Implements an triangular three-node constant strain plane-stress finite element. Each node has 2 degrees of freedom. The node numbering is anti-clockwise. The element features are summarized in Table 10.

 Keyword trplanestress2d Description 2D linear triangular isoparametric plane stress element Specific parameters - Unknowns Two dofs (u-displacement, v-displacement) are required in each node. Approximation Linear approximation of displacements and geometry. Integration Integration of membrane strain terms using one point gauss integration formula. Features Nonlocal constitutive support, Edge load support, Geometric nonlinearity support, Adaptivity support. CS properties Cross section thickness is required. Loads Body loads are supported. Boundary loads are supported and are computed using numerical integration. The side numbering is following. Each i-th element side begins in i-th element node and ends on next element node (i+1-th node or 1-st node, in the case of side number 3). The local positive edge x-axis coincides with side direction, the positive local edge y-axis is rotated 90 degrees anti-clockwise (see fig. (7)). Nlgeo 0, 1. Status Reliable

Table 10: trplanestress2d element summary

##### 2.4.4 QTrPlStr

Implementation of quadratic six-node plane-stress finite element. Each node has 2 degrees of freedom. Node numbering is anti-clockwise and is shown in fig. (8). The element features are summarized in Table 11.

 Keyword qtrplstr Description 2D quadratic triangular plane stress element Specific parameters [NIP #(in)] Parameters NIP: allows to set the number of integration points Unknowns Two dofs (u-displacement, v-displacement) are required in each node. Approximation Quadratic approximation of displacements and geometry. Integration Full integration using gauss integration formula in 4 points (the default) or in 7 points (using NIP parameter). Features Adaptivity support (error indicator). CS properties Cross section thickness is required. Loads Boundary loads are supported. Nlgeo 0, 1. Status -

Table 11: qtrplstr element summary

##### 2.4.5 TrPlaneStrRot

Implementation of triangular three-node plane-stress finite element with independent rotation field. Each node has 3 degrees of freedom. The element features are summarized in Table 12.

The generalization of this element, that can be positioned arbitrarily in space is trplanestrrot3d element. This element requires 6 degrees of freedon in each node. The element features are summarized in Table 13.

The implementation is based on the following paper: Ibrahimbegovic, A., Taylor, R.L., Wilson, E. L.: A robust membrane qudritelar element with rotational degrees of freedom, Int. J. Num. Meth. Engng., 30, 445-457, 1990. The rotation field is defined as ω = ( ) = uu. The following form of potential energy functial is assumed:

where τ is pseudo-stress (component of anti-symmetric stress tensor) working on dislocation (uu ω); the following constitutive relation foris assumed: τ = G(uu ω), where G is elasticity modulus in shear.

 Keyword trplanestrrot Description 2D linear triangular plane stress element with rotational DOFs Specific parameters [NIP #(in)] [NIPRot #(in)] Parameters NIP: allows to set the number of integration points for integration of membrane terms. NIPRot: allows to set the number of integration points for integration of terms associated to rotational field. Unknowns Three dofs (u-displacement, v-displacement, z-rotation) are required in each node. Approximation Linear approximation of displacements and geometry. Integration Integration of membrane strain terms using gauss integration formula in 4 points (default) or using 1 or 7 points (using NIP parameter). Integration of strains associated with rotational field integration using 1 point is default (4 and 7 points rules can be specified using NIPRot parameter). Features - CS properties Cross section thickness is required. Loads - Nlgeo 0. Status -

Table 12: trplanestrrot element summary

 Keyword trplanestrrot3d Description 3D linear triangular plane stress element with rotational DOFs Specific parameters [NIP #(in)] [NIPRot #(in)] Parameters NIP: allows to set the number of integration points for integration of membrane terms. NIPRot: allows to set the number of integration points for integration of terms associated to rotational field. Unknowns Six dofs (u-displacement, v-displacement, w-displacement, x-rotation, y-rotation, z-rotation) are required in each node. Approximation Linear approximation of displacements and geometry. Integration Integration of membrane strain terms using gauss integration formula in 4 points (default) or using 1 or 7 points (using NIP parameter). Integration of strains associated with rotational field integration using 1 point is default (4 and 7 points rules can be specified using NIPRot parameter). Features - CS properties Cross section thickness is required. Loads - Nlgeo 0. Status -

Table 13: trplanestrrot3d element summary

##### 2.4.6 TrPlaneStressRotAllman

Implementation of triangular three-node plane-stress with nodal rotations. Each node has 3 degrees of freedom. The element features are summarized in Table 14.

The generalization of this element, that can be positioned arbitrarily in space is trplanestressrotallman3d element. This element requires 6 degrees of freedon in each node. The element features are summarized in Table 15.

The implementation is based on the following paper: Allman, D.J.: A compatible triangular element including vertex rotations for plane elasticity analysis, Computers & Structures, vol. 19, no. 1-2, pp. 1-8, 1984. The element is based on plane stress element with quadratic interpolation. The displacements in midside nodes are expressed using vertex displacements and vertex rotations (for edge normal displacement component); the tangential component is interpolated from vertex values. For particular element side starting at i-th vertex and ending in j-th vertex the normal and tangential displacements at edge midpoint can be expressed as

where l is edge length. This allows to express global displacements in element midside nodes using vertex displacements and rotations. For a single edge, one obtains:

 Keyword trplanestressrotallman Description 2D linear triangular plane stress element with rotational DOFs Specific parameters Unknowns Three dofs (u-displacement, v-displacement, z-rotation) are required in each node. Approximation Linear approximation of geometry, quadratic interpolation of displacements. Integration Integration of membrane strain terms using gauss integration formula in 4 points. Zero energy mode The zero energy mode (equal rotations) is handled by adding additional energy term preventing spurious modes. Features - CS properties Cross section thickness is required. Loads - Nlgeo 0. Status -

Table 14: trplanestressrotallman element summary

 Keyword trplanestressrotallman3d Description 2D linear triangular plane stress element with rotational DOFs Specific parameters Unknowns Six dofs (D_u, D_v, D_w, R_x, R_y, R_z) are required in each node. Approximation Linear approximation of geometry, quadratic interpolation of displacements. Integration Integration of membrane strain terms using gauss integration formula in 4 points. Zero energy mode The zero energy mode (equal rotations) is handled by adding additional energy term preventing spurious modes. Features - CS properties Cross section thickness is required. Loads - Nlgeo 0. Status -

Table 15: trplanestressrotallman3d element summary