The entries under Support Reactions in the Results navigator allow you to control, which components are displayed graphically in the work window. They can be related to the local axes of rotated supports or to the global axis system XYZ. Table 4.3 shows the support forces and moments in numerical form.
If the structure is a 2D model, RFEM only displays the table columns of support forces and moments that are relevant for a planar structural system.
To display the support reactions of a particular load case, select the load case from the list in the main toolbar or the toolbar of the table.
The support forces are listed by lines. The x-locations shown in the table column represent the spacings of FE nodes along the line. They are related to the start node of the line. The surface grid is not relevant for line support forces.
The support forces are listed in three table columns where they are sorted by lines. The forces can be related to the global axes X, Y, and Z or the local axes X', Y', and Z' of the line supports. The axis reference in the table is controlled by settings in the Results navigator (see figure on the left).
The table shows the forces that are introduced into the support. Thus, with regard to signs, the table does not show the reaction forces on the part of the support. If support forces refer to the global coordinate system, the signs result from the directions of the global axes. If the global axis Z is directed downwards, the load case self-weight, for example, results in a positive support force pZ and a wind load against the global axis X results in a negative support force pX. Thus, the support forces shown in the table represent foundation loads.
If the local support forces pX', pY', and pZ' are displayed, the forces refer to the axes of the line supports X', Y', and Z'. Thus, the signs in the table for the introduced forces result from the directions of the local support axes. Use the Display navigator or the shortcut menu of line supports to display these axes.
The green vectors displayed in the graphic of the work window show the reaction forces on the part of the supports. The components of the support reactions are visualized by the size and direction of the vectors.
The support moments are listed in three table columns where they are sorted by lines. The moments are either related to the global axis system XYZ or the local axis system X'Y'Z' of the line support. If you have set a local reference, the support moments are labeled mX', mY', and mZ'.
The table shows the moments that are introduced into the support. As for support forces, the table does not show the reactions on the part of the support in regards to signs.
In the work window, however, reaction moments are shown on the part of the support. In addition to the vector display, an arc display can be set. To change the type of display, go to the menu and select Options → Display Properties → Edit (see Figure 8.5).
For load cases and load combinations, RFEM displays check sums of loads and support reactions at the end of the table. They are always related to the global axis system. Differences will occur between ∑ Forces and ∑ Loads if the model additionally has nodal supports and members/surfaces with elastic foundations. The ∑ Forces in these tables must therefore also be considered for the total summary.
The result diagrams of line supports can be specifically evaluated in a new window: Right-click the (selected) line support(s) and then select the Result Diagrams option in the shortcut menu (see Figure 8.12 in the left margin).
For more detailed information about the Result Diagram window, see Chapter 9.5.
In the work window, additional information is available for each line support:
- ∑ : Sum as resultant force
-
Φ : Mean value -
x : Distance of line's midpoint from line start -
e : Eccentricity of resultant force related to the line's midpoint -
M : Moment due to eccentricity of resultant force
To display this information, select Results → Support Reactions → Info in the Display navigator.
Note
The Z components of nodal and line support forces from another RFEM model can be applied as loads to the current model. This allows you to transfer loads from floor to floor to analyze 2D floor slabs, for example.
The support forces are imported into the current load case. Hence, it might prove to be advantageous to first create a load case for the new loads.
To open the import dialog box, go to the menu and select
- Tools → Import Support Reactions as Load.
First, specify the relevant model in the Import from dialog section. The button shown on the left helps you to select the right model. Then, RFEM imports the calculated load cases, load combinations, and result combinations you have to make the next decision for. When a RC is set, you also have to define whether you want to import the maximum or the minimum support forces.
If you do not want to import All support forces, you can specify the numbers of the relevant nodes, lines, and surfaces or select them graphically in the original model with the 
button.
In the Apply as Load in Current Model on dialog section, enter the numbers of the surfaces for which you want to create the loads or select them graphically using .
If the original and target surfaces lie exactly on top of each other, no entry is required in the Offset dialog section. Otherwise, you can use the text boxes to define the global offsets ΔX and ΔY for the import. They refer to the global axes.
In the Line Supports dialog section, you can choose whether the support forces are imported as free line loads with a uniform (averaged) or a polygonal (actual) load distribution.
For result combinations, it is possible to adjust the default setting for the extreme values shown in the results table by using the menu option
- Table → View → Result Filter
or the corresponding button in the table toolbar shown on the left.
The check boxes in the Table Filter dialog box control the type and extent of the numerical output.