This page contains frequently asked questions related to shell elements.

General

What are the practical limits on the maximum thickness of shell elements relative to the shell dimension?

When using the thick plate formulation, both the bending and the shear deformations are accurately (within the assumptions of the formulation) accounted for. I have attached verification example 2-012 in which 0.1 in x 0.1 in shell elements with 0.5 in thickness are used and the solution obtained from SAP2000 exactly matches independent solution.

As a general rule, one would expect that thick-plate effects would become important when the span to thickness ratio is about 20:1 to 10:1, and the adequacy of the formulation would be good for a ratio of down to about 5:1 or 4:1. Note that this is the span of deformation we are talking about here. As the elements are meshed, the elements may actually be thicker than the plan dimension, and that is OK. The important thing to consider is the ration of the span of deformation to thickness.

However, please note that all shell elements are approximate and a special case of three-dimensional elasticity. Depending on your specific needs, shell elements may be appropriate, but for some other types of analyses (such as assessment of local behavior) you may obtain more accurate response by using solid elements. You can always set up simple test problems to check the difference between different modeling approaches.

Could you explain the difference between thick shell and thin shell elements?

The two thickness formulations for area section, available in SAP2000, determine whether or not transverse shearing deformations are included in the plate-bending behavior of a plate or shell element:

• The thick-plate (Mindlin/Reissner) formulation includes the effects of transverse shear deformation
• The thin-plate (Kirchhoff) formulation neglects transverse shearing deformation

Shearing deformations tend to be important when the thickness is greater than about one-tenth to one-fifth of the span. They can also be quite significant in the vicinity of bending-stress concentrations, such as near sudden changes in thickness or support conditions, and near holes or re-entrant corners. Even for thin-plate bending problems where shearing deformations are truly negligible, the thick-plate formulation tends to be more accurate, although somewhat stiffer, than the thin-plate formulation. However, the accuracy of the thick-plate formulation is more sensitive to large aspect ratios and mesh distortion than is the thin-plate formulation.

It is generally recommended that you use the thick-plate formulation unless you are using a distorted mesh and you know that shearing deformations will be small, or unless you are trying to match a theoretical thin-plate solution. The thickness formulation has no effect upon membrane behavior, only upon plate-bending behavior.

As a general rule, the contribution of shear deformations becomes important when the span to thickness ratio is about 20:1 to 10:1, and the adequacy of the formulation would be good for a ratio of down to about 5:1 or 4:1. Note that this is the span of deformation. As the elements are meshed, the elements may actually be thicker than the plan dimension, and that is OK. The important thing to consider is the ration of the span of deformation to thickness.

I have area object with more than 4 vertices and I have not specified any meshing. However the analysis model shows mesh. How was this mesh created?

It no auto-meshing has been assigned to an area object that has been drawn using more than 4 nodes, the program will use general meshing tool to mesh such areas.

What is the difference between "Uniform (Shell)" and "Uniform to Frame (Shell)" loads

When using the "Uniform (Shell)" option, the uniform loads are applied directly to the shell elements and are transferred to the structure via the joints of the shell element.

When using the "Uniform to Frames (Shell)" option, the uniform loads are applied directly to the frame elements defined along the edges of the shell under consideration. You can define one way or two way load distribution. Please note that you can review how the "Uniform" to Frames loads are distributed to the frame elements in your model by using "Display > Show Load Assigns > Area" menu command.

How can I model simply supported slab using shell elements?

Please see the Modeling simply supported shells tutorial.

How can I post-process area output (the area is used to model bridge diaphragm) to get meaningful design forces?

You could obtain diaphragm design forces from joint forces of the shells used to model the diaphragms. These shell joint forces would need to be transformed to the location of interest. Please note that the program uses this procedure to obtain section cut forces; using section cuts to obtain the design forces would, therefore, be another alternative.

How are stresses for the shell elements calculated? Can I compare the calculated stresses directly to the allowable stress of shell material?

Yes, the shell stresses obtained from SAP2000 can be directly compared to the allowable stress of the material. You can display the shell stresses by right-button click on the shell elements when the stresses are displayed or by reviewing the stresses in a tabular format via "Display > Show Tables > ANALYSIS RESULTS > Element Output > Area Output > Table: Element Stresses - Area Shells".

The stresses are calculated as a product of stress-strain constitutive matrix and strain vector which is obtained from joint displacements. The procedure is not based on a simple formula, but rather on several techniques described in the following references cited in the CSI Analysis Reference Manual:

• A. Ibrahimbegovic and E. L. Wilson: "A Unified Formulation for Triangular and Quadrilateral Flat Shell Finite Elements with Six Nodal Degrees of Freedom," Communications in Applied Numerical Methods, Vol. 7, pp. 1--9, 1991

• R. L. Taylor and J. C. Simo: "Bending and Membrane Elements for Analysis of Thick and Thin Shells," Proceedings of the NUMEETA 1985 Conference, Swansea, Wales, 1985

The above references are available in the open literature.

A comprehensive description can also be found in Prof. E. L. Wilson’s book available from CSI at http://orders.csiberkeley.com/ProductDetails.asp?ProductCode=ELWDOC-3D.

See page Shell element formulation DRAFT for additional details.

How does the program apply stiffness modifiers for shell elements?

When stiffness modifiers are applied, the corresponding terms in the stiffness matrix of the shell element will get modified. You could also look at this as reducing (or increasing) the Young's or shear moduli of the material for the given directions. The stiffness matrix for the entire structure is then assembled and the equilibrium equations are solved to find the unknown displacements. The displacements are then used to calculate the internal forces and stresses.

Layered Shell Element

Can you explain the coupling of membrane and plate behavior for nonsymmetrical layering?

Extended Question: The CSI Analysis Reference Manual states: "Unless the layering is fully symmetrical in the thickness direction, membrane and plate behavior will be coupled". If the element is defined such that planes remain plane in the thickness direction, then even for a symmetric definition of membrane layers, the layers would contribute to the out of plane bending stiffness and see stresses when there is rotations in the plate element. Am I missing something here?

Answer: You are correct that the membrane layers contribute to bending. The statement here regards whether or not transverse loading generates membrane forces/deformation, and likewise whether or not in-plane loading generates bending. The coupling effect could be demonstrated by applying uniform temperature load to the shell element. For symmetrical layering, the temperature load will cause only in plane deformations. For nonsymmetrical layering, out-of-plane deformations will be generated. This is similar to bi-metal strip, illustrated in this Wikipedia article: http://en.wikipedia.org/wiki/Bi-metallic_strip

Could you please explain how the material orientation is related to the element orientation?

Extended Question: It is not clear how the material orientation and the S11, S22, and S12 orientation are defined for the elements. Are the 1, 2, and 3 directions the same as the local axes for the shell element, that can be seen as red, white, and blue colors on the screen? In the "Nonlinear Shear Wall" movie, for longitudinal bar elements, a material angle of 90 degrees is used and then the nonlinearity is defined in the S11 direction, which is the horizontal direction for the element. This suggests that internally, the program is rotating the local axis for that layer by 90 degrees relative to the element local axis. Is that the right interpretation? Would it have the same effect to have the material at zero degrees, but define the nonlinearity in the S22 direction? On the other hand, if the angle is just referring to material orientation, should not the nonlinearity be defined in the S22 direction which is the nonlinear direction?

Answer: As shown in our the figures below (the first one was taken from our manual, while the second one was taken from the video), the material orientation in a given layer is defined relative to the material local coordinate system by specifying a material angle. Using material angle of 90 degrees and specifying the nonlinearity in S11 direction has the same effect as using material angle of 0 degrees and specifying the nonlinearity in S22 direction. For uniaxial materials like rebar, whose behavior is only defined in the material 1 direction, you must use the former specification. For fiber-wrapped composites, you may want to specify material behavior at other some angle, say 45 degrees, to the element local axes. Note that loading and the output forces/stresses will always be in the element axes, even though you may specify material properties in the material coordinates.