#303 Stress calculations in QUAD elements (Gaussian points and nodal points): Elemental stress, Nodal stress

For QUAD elements with shapes deviating significantly from perfect rectangle stresses are indeed most realistic at Gauss points.

The primary purpose of using Gauss integration points is numerical integration. These points are chosen so that the results for a particular numerical integration scheme are the most accurate. (the Gauss Quadrature for n-th order of integration). At the solution phase, the solver evaluates the [B] matrix while building the element stiffness matrix and the global stiffness matrix. When during postprocessing nodal DOFs vector {u} is used to calculate stresses and strains using the following formulas: strain

and stress

at the Gauss points. It saves the effort of evaluating [B] matrices again. The stresses are the most accurate at Gauss points, so we take stresses at the integration points and extrapolate them to get stresses at element nodes. The element centroid values are the average of nodal values.

In the stiffness method of solution, the stresses are obtained from the computed displacements and thus are derived quantities. The accuracy of derived quantities is generally lower than that of primary quantities (the displacements). For example, if the accuracy level of displacements is 1% that of the stresses may typically be 10% to 20%, and even lower at boundaries.

It is important to realize that the stresses computed at the same nodal point from adjacent elements WILL NOT GENERALLY BE THE SAME since stresses are not required to be continuous in displacement-assumed finite elements. This suggests some form of stress averaging can improve stress accuracy.

To compute elemental nodal stresses, we evaluate stresses {sigma} at the Gauss integration points used in the element stiffness integration rule and then extrapolate to the element node points.

The stresses computed in the element-by-element fashion by extrapolation will generally exhibit jumps between elements. For printing and plotting purposes(!!!), it is usually convenient to “smooth out” those jumps by computing averaged nodal stress. This averaging may be done in two ways:

1) Unweighted averaging: assign the same weight to all elements that meet at a node.
2) Weighted averaging: the weight assigned to element contributions depends on the stress component and the element geometry and possibly the element type.

Altair OptiStruct Stress Output Options:

1. CENTER = element stresses for shell and solid elements are output at the element center only.
2. CUBIC = element stresses for shell elements are output at the element center and grid points using the strain gauge approach with cubic bending correction.
3. SGAGE = element stresses for shell elements are output at the element center and grid points using the strain gage approach.
   CORNER or BILIN = element stresses for shell and solid elements are output at the element center and grid points using bilinear extrapolation.
4. GAUSS = element stresses for shell and solid elements are output at the element center and the Gauss integration points.

 

Nastran Stress Output Options:

1. CENTER = Requests CQUAD4, CQUADR, and CTRIAR element stresses at the center only. The default for CQUAD4 is CENTER. The default for CQUADR and CTRIAR is CORNER.
2. CUBIC = Requests CQUAD4 element stresses at the center and grid points using strain gage approach with cubic bending correction.
3. SGAGE = Requests CQUAD4 element stresses at center and grid points using strain gage approach.
   CORNER or BILIN = Requests CQUAD4, CQUADR, and CTRIAR element stresses at the center and grid points using bilinear extrapolation.

The program obtains the stresses at the nodes of the element by extrapolation of the results calculated at the Gaussian points. After solving the problem, the nodal stress results at each node of each element are available in the database. Therefore, there will be MULTIPLE stress results at nodes common to two or more elements (as many as elements go to the same node). These results will be different from each other since the Finite Element Method is an approximate method. For example, if a node is common to 4 elements, there will be four slightly different values ​​for each stress component at the node. During the results display, the user can choose between stresses at nodes or elements.

During the post-processing of stresses at nodes, the program averages the corresponding results of all the elements that contribute stresses to said node. For example:

During element stress post-processing, the program averages the corresponding nodal stresses for each element. Using the same example:

A single node shared by multiple quad elements can have different stress values reported for each element, meaning the stress at that node can appear different depending on which element you are looking at; this is because each element calculates its own stress based on its internal strain distribution and the nodal displacements, which can vary slightly between elements even at the shared node.

Notes:

1. Due to the different “averaging” methods, the maximum values ​​obtained at nodes and elements are different. In the example above, the maximum stress value at nodes is 5.0, and the maximum stress value at elements is 5.66.
2. If the mesh is “slightly dense” compared to the variation gradient of the results, then the maximum stress values ​​at nodes and elements will be very different.
3. Comparing the maximum values ​​in nodes and elements is a good indicator of the degree of mesh refinement used in the areas of maximum stress concentration.