Members are attributes of lines. By assigning a cross-section (which also defines a material), the member receives a stiffness. When generating the FE mesh, 1D elements are created on members.
Members can only be connected with each other on nodes. When members cross each other without sharing a common node, no connection exists. No internal forces are transferred on such crossings.
Graphically, you can apply members as Single, Continuous, or to already existing Lines. The Inserted Member option is described in Chapter 11.4.13.
Enter the number of the line with member properties into the text box of the dialog box or the column in the table. In the New Member dialog box, you can also select the line graphically.
The start and end nodes of the line define the member orientation, which also affects the position of the member's local coordinate system (see "member rotation" in this chapter). The member orientation can quickly be changed in the graphic: Right-click the member and select Reverse Member Orientation in the shortcut menu.
The member type allows you to define the way internal forces are absorbed, or which properties are assumed for the member.
Different options are available for selection in the Member Type list. Each member type has an assigned Color that can be used to display different kinds of members in the model. Colors are controlled in the Display navigator with the Colors in Rendering According to option (see Chapter 11.1.9).
|Member Type||Short Description|
Bending-resistant member that can transmit all internal forces
Coupling member with rigid stiffness
Downstand beam considering the effective slab width
Beam with moment hinges at both ends
Truss (only N)
Member with stiffness E ⋅ A only
Truss (only N) with failure in case of compression force
Truss (only N) with failure in case of tension force
Truss (only N) with failure when compression force > Ncr
Member that only transfers tension forces. Calculation is performed according to the large deformation analysis.
Cable on Pulleys
Member on polyline, can only be shifted in longitudinal direction, absorbing only tensile forces (pulley)
Member for integration of surface, solid, or member results
Member with user-defined stiffnesses
Rigid coupling with bending-resistant connections at both ends
Rigid coupling with bending-resistant connection at member start and hinged connection at member end
Rigid coupling with hinged connections at both ends (only axial and shear forces are transmitted, but no moments)
Rigid coupling with bending-resistant connection at member end and hinged connection at member start
Member with spring stiffness, definable activity zones, and damping coefficients
Member that is ignored in the calculation
A beam does not have any releases defined on its member ends. When two beams are connected with each other and no release has been defined for the common node, the connection is bending-resistant. Beams can be stressed by all types of loads.
This member type couples the displacements of two nodes with a rigid connection. Thus, in principle, it corresponds to a Coupling member. You can use a rigid member to define members with a high stiffness while considering hinges that may also have spring constants and nonlinearities. Hardly any numeric problems occur, as the stiffnesses are adjusted to the system. RFEM also shows internal forces for rigid members.
The following stiffnesses are assumed (also applies for couplings and Dummy Rigids):
- Longitudinal and torsional stiffness:
- Flexural resistance:
- Shear stiffness (if activated):
Due to this type of member, it is no longer necessary to define a Dummy Rigid (see Chapter 4.13) and assign it as a cross-section.
Ribs are described in Chapter 4.18.
This type of a truss member absorbs axial forces in the form of tension and compression. A truss member has internal moment hinges on its member ends. Therefore, an additional release definition is not allowed. RFEM only shows node internal forces (which are transferred to the connecting members). The member itself shows a linear distribution of internal forces. An exception is the concentrated load on the member, which means that no moment diagram is visible as a result of self-weight or a line load. The boundary moments are zero because of the release; a linear distribution is assumed along the member. The nodal forces, however, are calculated from the member loads, which guarantees correct transmission.
The reason for special treatment is that a truss girder, according to general understanding, only transfers axial forces. Moments are of no interest. Therefore, they are deliberately not shown in the output, nor are they calculated as a part of the design. To display moments from the member loads, use the member type Truss.
For the member type Truss (only N), buckling perpendicular to the principal axes is not possible. Effects of member buckling are therefore not considered in the calculation!
A tension member can only absorb tension forces, and a compression member only compression forces. The calculation of a framework structure with these types of members is carried out iteratively: In the first iteration, RFEM determines the internal forces of all members. If tension members have negative axial forces (compression), or if compression members have positive axial forces (tension), an additional iteration step is started in which the rigidity of these members is no longer considered - they have failed. This iteration process continues as long as tension or compression members fail. Depending on modeling and loading, a system may become unstable due to failure of tension or compression members.
A failed tension or compression member can be considered again in the stiffness matrix if it is reactivated in a later iteration step due to redistributions in the system. In the menu, select Calculate → Calculation Parameters to open the Global Calculation Parameters dialog tab where you can set the Reactivation of Failing Members. You can find detailed information about these functions in Chapter 7.3.
A buckling member absorbs unlimited quantities of tensile forces. Compressive forces, however, can only be absorbed until the critical Euler load is reached.
With this type of member, you can often avoid instabilities that occur in nonlinear calculations according to the second order theory or large deformation analysis due to buckling of truss members. If you realistically replace trusses by buckling members, the critical load is increased in many cases.
Cables only absorb tension forces. They are used to analyze cable chains with longitudinal and transversal forces through iterative calculation and by taking the cable theory into account (large deformation analysis - see Chapter 7.3.1). For that purpose, it is required to define the complete cable as a cable chain consisting of several cable members.
To quickly create a catenary, go to the menu and select Tools → Generate Model - Members → Arc (Chapter 11.7.2). The more accurately the starting shape of the catenary corresponds to the real cable chain, the more stable and the faster you can perform the calculation.
It is recommended to prestress cable members in order to prevent compression forces that would result in failure. Furthermore, cables should only be used if deformations have a considerable part in changes of the internal forces, that is, when large deformations can occur. For simple, straight riggings such as transverse bracings (projecting roof), tension members are completely sufficient.
When evaluating deformations of cable members, set the scaling factor in the control panel (see Figure 3.19) to "1" so that tightening effects are represented realistically.
This cable type only absorbs tensile forces and is calculated according to the cable theory (large deformation analysis). In contrast to a cable, it can only be applied to a polyline with at least three nodes. This member type is suitable for flexible tension elements whose axial forces are passed on by means of deviating points (e.g. pulley).
In contrast to a normal cable member, only a displacement within the internal nodes in the longitudinal direction ux is possible. The member must therefore not be stressed by member loads acting in the local directions y or z.
The displacement in longitudinal direction is not allowed to be free at the ends of the cable.
For the internal nodes of the polyline, it does not matter whether a nodal support is available or if the member is connected to another construction: RFEM analyzes the total model of the cable member along the length of the polyline.
For members of the member type Cable on Pulleys, RFEM only considers displacements ux and axial forces N.
Like a cut through the model, a result beam can be placed anywhere in the model as a virtual member. Use it to display the internal forces of surfaces, members, and solids in the form of integrated results. This allows you, for example, to read the resulting shear forces of a surface used for masonry design in the display.
The result beam requires neither a support nor a connection to the model. It is not possible to apply loads to a result beam.
The integration parameters must be set in a dialog box (see Figure 4.162) that you open by using the [Edit] button.
In the Integrate Stresses and Forces dialog section, define the result beam's zone of influence. The dialog graphic illustrates the parameters relevant for the individual options.
The Include Objects dialog section allows for a specific selection of model elements whose results should be taken into account for the integration: surfaces, solids, members.
When the result beam is defined, you can activate and deactivate the display of integration areas in the Display navigator (see figure shown on the left).
The member stiffnesses can be directly specified in a dialog box that you open with the [Edit] button. Thus, the assignment of a cross-section is unnecessary.
To display the definition of the stiffness matrix, use the [Info] button.
A coupling member is a virtual, very stiff member with definable rigid or hinged properties. It is possible to couple the degrees of freedom of the start and end nodes in four different ways. The axial and shear forces, or torsional and bending moments, are transferred directly from one node to the other. Couplings can be used to model special situations for the transfer of forces and moments.
RFEM calculates stiffnesses of couplings depending on the model in order to exclude numerical problems.
With the Rigid variant, you can also define coupling members while considering springs and nonlinearities of releases.
To control the display of coupling results, use the Display navigator.
If Spring members are set, you can open a new dialog box by using the [Edit] button or in the table.
Define the spring properties via Parameters or in a Diagram. The spring constant C1,1 describes the stiffness of the member in its local x-direction according to the following relation:
The Slippage specifies a zone of the deformation where the spring does not absorb any forces.
You have two options for defining the spring Limits:
- Deformation: The values umin and umax define the geometric activity zone of the spring. The spring acts as a rigid member (stop) for deformations outside the specified zone.
- Force: The values Nmin and Nmax define the activity zone for the forces that can be absorbed by the spring. If the axial force is beyond the defined limits, the spring fails.
Use the Diagram tab to define spring properties more precisely. These settings are largely identical with the parameters available for nonlinear member releases (see Chapter 4.14).
A dummy member with its loads is not considered in the calculation. Use dummy members to, for example, analyze changes in structural behavior if certain members are not effective. You do not need to delete these members; their loading is kept as well.
The two text boxes or table columns are used to define the cross-sections for the member start and end. The cross-section numbers refer to the entries in Table 1.13 Cross-Sections (see Chapter 4.13). Assignment is made easier by colors related to different cross-sections.
When you enter different numbers for the start and end cross-section, a taper is created. RFEM interpolates the variable stiffnesses along the member according to polynomials of a higher grade. Input of nonsense such as a taper consisting of an IPE cross-section and a round steel will be identified by the plausibility check before the calculation starts.
The internal determination of tapered cross-section values is controlled by the Taper Shape set in the Options tab, or the corresponding table column (see Chapter 4.17).
The member-related coordinate system xyz is defined clockwise by right angles. The local axis x always represents the centroidal axis of the member, connecting the start node with the end node of the line (positive direction). Member axes y and z, or u and v for asymmetrical cross-sections represent the principal axes of the member.
The position of the local axes y and z is set automatically: Axis y is perpendicular to the longitudinal axis x and parallel to the global plane XY. The position of the axis z is determined by the right-hand rule. The z' component of the z-axis is always pointed "downwards" (i.e. in direction of the gravity), irrespective of whether the global axis Z is oriented downward or upward.
To check the member position, use the 3D rendering. You can also use the Display navigator or the member shortcut menu to display the Member Axis Systems x,y,z.