The primary results in the Beam interface are the section forces: axial force, shear forces, bending moment, and twisting moment. The shear forces and bending moments are oriented along the principal directions as described in the Section Orientation node.

In the Quality section of the plot, you can control the level of averaging by changing the Smoothing method.

The default method is Inside material domains. In the Beam interface, two adjacent edges are considered as part of the same material domain only if they share both material and cross-section data. In many cases this gives an optimal level of smoothing since beams that meet at nonzero angles often have different cross sections.

You may however want to use Inside geometry domains instead as smoothing method. This means that there will be no smoothing at points where a connection may occur.

Evaluation of stresses in beam elements required special consideration since the stress field produced by various section forces have different distributions over the cross section. All that is known in the beam formulation is the peak value of each stress contribution. Details about how stresses are combined are given in the section Stress Evaluation. In general, the different contributions to the total stress are combined in a conservative manner. If you need to study the stress distribution over the cross section in detail, this can be done using the Beam Cross Section interface.

A common representation of beam results is to draw diagrams of shear forces and bending moments on top of the structure. Such diagrams are generated as predefined plots, and you can add them from the Add Predefined Plot window. They are available as the group Section Force Diagrams.

The section force diagrams do not use the standard variables for shear forces and bending moments. These variables, like beam.Tzl and beam.Myl, are constant and linear, respectively, within each element, as an effect of the finite element formulation. Rather, a set of variables that are augmented with information about distributed loads is used. The names of these variables are beam.Tzl_d and beam.Myl_d, for example. In essence, a numerical integration of the loads is performed along each element up to the position where a value is requested. The augmented variables have a much smoother distribution than the standard section forces.

The effect is that you can display good section force diagrams also with a very coarse mesh. It should however be noted that the numerical integration of the loads has a limited resolution. This is not a problem for smooth distributed loads, but if you would add a discontinuous line load with an expression like q0*(X>1.52[m])*(X<1.54[m]), the load integration may fail to capture it accurately if the element length is an order of magnitude larger than the 0.02 m over which the load is distributed. This is seldom a problem in reality, since such a mesh can be considered as too coarse, and may not even capture the true resultant of such a load.

The section force diagrams are constructed using Arrow Line plots and you may need to tune them for your model. Here are some hints on how to work with the section force diagrams: