Comparison of Plastic Design (Shell Model) and Nonlinear Member Model

Technical Article

The following example presents a comparison between a shell model and a simple member model performed in RFEM. In the case of the shell model, a beam is suspended within surfaces and modelled with restraints on both sides due to the boundary conditions. This is a statically indeterminate system that will form plastic hinges when overloaded. The comparison is carried out on a member model, which has the same boundary conditions as the shell model.

Figure 01 - Complete Model

Entering Shell Model

You can create the shell model in RFEM which provides the option to directly generate a member element into surfaces (function ‘Generate Surfaces from Member’). A member with the length of 4 m is initially created. The cross‑section type IPE 200 is selected. After modelling the beams, surfaces are generated from the member by using the function mentioned above.

Figure 02 - Generate Surfaces from Member

After creating a pure shell model of the beam, you can define the boundary conditions. The beam should be supported on both sides. These boundary conditions can be created with the use of line supports. For this application, the web and flanges of the surface model can be supported with line supports. A complete restraint of the support is not required as the restraint results from the limit of translational degrees of freedom on the web and the flange.

Figure 03 - Support Conditions

After entering the boundary conditions, you can define plastic behaviour of the surfaces by selecting the Isotropic Plastic 2D/3D material model. This material model allows you to consider the surface plastification during the calculation. In the same dialog box, you can also set the von Mises equivalent stress as the material’s yield strength is set to 24 kN/cm². When you specify the plastic behaviour of the material, the load increment is automatically activated in the calculation parameters. The load increment will contribute to more efficient convergence behaviour in the calculation.

Figure 04 - Material Model

A line load is applied to the structure at the intersection line between the upper flange and the web. The load magnitude is set to 45 kN/m. Plastic hinges begin to form at both supports.

Figure 05 - Load

After the calculation of the entire structure, the deformations are immediately available. It is possible to switch views to the equivalent stress according to von Mises. The default setting for RFEM displays the stresses with smoothed contours. This causes a distorted view of the results because the plastic maximum stress is exceeded. Therefore, it is necessary to select the display option ‘Constant on Elements’ for the internal forces and stresses on the surface. These results represent the mean value of each FE element. Node values of the FE element are used for the generation of the mean value. When using plastic or nonlinear material behaviour, it is always necessary to select the display option ‘Constant in Elements’. This allows for the plastic stress of the element to be displayed accurately after the plastic behaviour has occurred.

Figure 06 - Distribution of Internal Forces/Stresses

In order to perform the comparison with the analytical calculation, it is necessary to make the results of the surface model comparable to those of the analytical model. For this, it is possible to use a result beam. With a result beam, all surface or solid stresses in the model can be integrated together. A comparison with the analytical model can further be performed.

The member is defined in this model. When the 1D member is generated into a surface model, a dummy member appears in the location of the original member, which serves as a placeholder. This member has no stiffness and will not be considered in the calculation. You can change the member type from ‘Dummy’ to ‘Result Beam’. All surfaces can then be assigned to this result beam to view the internal forces as one resultant value. For this example, the flange and web surfaces are included in the result beam to view the elements’ internal force results as if it were a single member.

Figure 07 - Definition of Result Beam

Entering Member Model

For comparison, a simple member model is now created and loaded to form a plastic hinge. A simple member with an IPE 200 cross‑section is defined. For this member, we will create an added material with isotropic material properties. The steel type S235 is selected for this entry. There is the additional option to consider a plastic hinge under Member Nonlinearity. Since only a plastic moment release should be defined, all the other internal forces are set to a large value so they remain unaffected. The plastic limit moment for IPE 200 with S235 can be calculated by the following:

$$\begin{array}{l}{\mathrm M}_\mathrm{ply}\;=\;{\mathrm f}_\mathrm y\;\cdot\;{\mathrm W}_\mathrm{ply}\\{\mathrm M}_\mathrm{ply}\;=\;24\;\mathrm{kN}/\mathrm{cm}^2\;\cdot\;220.6\;\mathrm{cm}^3\;=\;54\;\mathrm{kNm}\end{array}$$

Figure 08 - Definition of Plastic Hinge

The boundary conditions are assumed to be restrained on both sides in order to compare the current model with the previous surface model. The load is applied as a member load in this example due to the fact that line loads can be used for surfaces only. The member load magnitude is set to 45 kN/m.

Evaluation of Comparative Calculation

The result of both calculations can now be compared in the graphic below. The results are almost identical. With the surface model, you can clearly see the plastic hinges which have formed on the supports. The resulting internal forces on the result beam are very similar to the internal forces of the member model which includes plastic hinges. The result differences can be attributed to the modelling of the surface model and the idealisation of the member model.

Figure 09 - Result Comparison



Contact us

Contact to Dlubal

Do you have questions or need advice?
Contact our free e-mail, chat, or forum support or find various suggested solutions and useful tips on our FAQ page.

+49 9673 9203 0

RFEM Main Program
RFEM 5.xx

Main Program

Structural engineering software for finite element analysis (FEA) of planar and spatial structural systems consisting of plates, walls, shells, members (beams), solids and contact elements

Price of First License
3,540.00 USD