Smoothing of Surface Internal Forces in RFEM
When calculating a surface model, the internal forces are determined separately for each finite element. Since the element-by-element results usually represent a discontinuous distribution, RFEM performs smoothing of the internal forces that takes into account the influence of adjacent elements. The discontinuous distribution of internal forces is adjusted with this method. The result evaluation is thus clearer and easier.
You can select different options in the program to display unsmoothed or smoothed results. They are described in the RFEM manual. Smoothing options to evaluate surface internal forces and stresses are also explained in this technical article. The following article uses an example to illustrate how the internal forces in finite elements for smoothing are used to determine the values. In addition to the position of a finite element, the plate theory - Mindlin or Kirchhoff - plays a role in this process.
Example: Plate According to Mindlin and Kirchhoff
A plate with the dimensions 4 m ⋅ 3 m is created as a two-dimensional model. The plate is hinged on both sides to the shorter boundary lines. The rotation of the longer boundary lines is restrained by a restraint. To avoid transversal strain effects, Poisson's ratio of the material is set to zero. To compare the determination of internal forces according to the plate-bending theories of Kirchhoff and Mindlin, a plate thickness of 80 cm is selected. Thus, the ratio d/L = 0.2 is given in the limit zone between the two bending theories (see https://www.dlubal.com/en/support-and-learning/support/faq/003158).
To keep it simple, the mesh size of the FE mesh is set to 1 m. Thus, there are 4 ⋅ 3 finite elements.
A load of p = 5 kN/m² acts on the plate. The self-weight is not applied in the load case.
Unsmoothed Internal Forces
The results of the computation kernel for the internal forces vx and mx are considered for a longitudinal section running in the center of the plate. The distribution of the unsmoothed internal forces element by element can be represented by the "Not Continuous" display option. According to the bending theories of Mindlin and Kirchhoff, the diagrams shown in Figure 02 are available.
Standard Smoothing for Internal Nodes
For FE nodes that lie within a surface, the arithmetic mean is first formed from the nodal values of the adjacent finite elements. For this approach, the elements must lie in a surface and on the same side of a possible internal line. The node must not be a user-defined node in the surface.
For the location of discontinuity at x = 1.00 m, these values are the following internally (the result of this step is not available for the output).
Smoothing for Edge Nodes
At the edges of a surface ("Continuous within surfaces" smoothing option) or a model ("Continuous Total"), there are no adjacent finite elements that could be used for averaging the nodal values. Therefore, a different approach is used, which is performed in two steps.
In the first step, the averaged values are calculated for those nodes that are not located on the edge of a surface or the model. The values of the nodes at the edges are calculated in such a way that the original values remain in the centers of the finite elements. In the second step, the averaged values for the edge nodes are determined.
The following values result for the edge node at x = 0.00 m.
According to Mindlin, the shear forces are calculated as the first derivative of the deflection.
These values are determined by the calculation kernel and used directly. The smoothing of shear forces is then carried out as described above, depending on the position of the FE node in the surface.
In the bending theory according to Kirchhoff, the shear forces are calculated as the third derivative of the deflection.
This value determination using the third derivative results in a considerable loss of accuracy. For this reason, the shear forces of the computation kernel are not used, but determined from the derivations of the moments by an improved approach.
The moments mx, my, and mxy in the equations represent the smoothed values that are determined according to the methods described above. This results in more accurate values for the shear forces than calculating them with the computation kernel.
While the moment values in the integration points correspond to the theoretical values, the extrapolation leads to a loss of accuracy when using the hyperbolic paraboloid function for smoothing. A hyperbolic paraboloid only approximates the moment distribution in the element. For this reason, an improved algorithm is used that replaces the extrapolation with an advanced shear force integral method. Since the distribution of shear force in the surface element is assumed to be the shape of a hyperbolic paraboloid (surface of the second order), the integral of this surface represents a surface of the third order, which displays the moment distribution with greater accuracy.
This approach corresponds to the equations described above for determining the shear forces via the derivatives of the moments. The moments are then determined with the following equations.
The integration constants mx,0 and my,0 are calculated from the conditions of the value in the center of the member.
S represents the surface of the element.
The values of the internal forces are determined by the methods described above; the integrals, by a numerical integration. The moments thus determined are then smoothed according to the method for internal nodes or edge nodes.
In the bending theory according to Mindlin, the following values result in this example.
The following values are obtained for the bending theory according to Kirchhoff.
In the smoothing process, the steps described above are performed gradually in the program. The smoothed values can be displayed graphically with the display option "Continuous within Surfaces".
Dipl.-Ing. (FH) Robert Vogl
Technical Editor, Product Engineering & Customer Support
Mr. Vogl creates and maintains the technical documentation. In addition, he is involved in the development of the SHAPE-THIN program and provides customer support.
Do you have any further questions or need advice? Contact us via phone, email, chat or forum or find suggested solutions and useful tips on our FAQ page, available 24/7.
RF-/JOINTS Timber - Timber to Timber Add-on Module for RFEM/RSTAB | Design of Direct Timber Connections According to Eurocode 5
RF-/JOINTS Steel - Column Base Add-on Module for RFEM/RSTAB | Hinged and Restrained Column Bases According to EC 3
RF-/STEEL Fatigue Members Add-on Module for RFEM/RSTAB | Fatigue Design of Members According to EN 1993-1-9
RF-/JOINTS Steel - Tower Add-on Module for RFEM/RSTAB | Hinged Connections of Lattice Towers According to EC 3
RF-/TOWER Effective Lengths Add-on Module for RFEM/RSTAB | Determination of Effective Lengths for Lattice Towers
RF-LOAD-HISTORY Add-on Module for RFEM | Consideration of Plastic Deformations from Previous Load Conditions
RF-/STEEL NBR Add-on Module for RFEM/RSTAB | Design of Steel Members According to ABNT NBR 8800: 2008
RF-/FE-LTB Add-on Module for RFEM/RSTAB | Lateral-Torsional Buckling Analysis According to Second-Order Analysis (FEM)
- Are the models and presentations from Info Day 2018 freely available, and can you send them to me?
- How can I display membrane stresses in the results of RF‑STEEL Surfaces?
- In RF‑CONCRETE Surfaces, I obtain a high amount of reinforcement in relation to a lever arm that is almost zero. How is such a small lever arm of internal forces created?
- How does the "Orthotropic Plastic" material model work in RFEM?
- I would like to define a line support with ineffective tension and apply the tension force on this line using a nodal support instead. Why does the line support still receive a tension force?
- When converting from the manual definition of reinforcement areas to the automatic arrangement of reinforcement according to Window 1.4, the result of the deformation calculation differs, although the basic reinforcement has not been modified. What is the reason for this change?
- Why do I get a discontinuous area in the distribution of internal forces? In the area of the supported line, the shear force VEd shows a jump, which does not seem plausible.
- How is it possible to make factorized combinations of a dead load in the context of form‑finding?
- Where can I find detailed information about orthotropy mentioned in the manual?
- I obtain different results when comparing the deformation analysis in the RF‑CONCRETE add-on modules and another calculation program. What could be the reason for this?
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