4.17 Members

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).

Table 4.7 Member types

Member Type	Short Description
Beam	Bending-resistant member that can transmit all internal forces
Rigid	Coupling member with rigid stiffness
Rib	Downstand beam considering the effective slab width
Truss	Beam with moment hinges at both ends
Truss (only N)	Member with stiffness E ⋅ A only
Tension	Truss (only N) with failure in case of compression force
Compression	Truss (only N) with failure in case of tension force
Buckling	Truss (only N) with failure when compression force > Ncr
Cable	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)
Result Beam	Member for integration of surface, solid, or member results
Definable Stiffness	Member with user-defined stiffnesses
Coupling Rigid-Rigid	Rigid coupling with bending-resistant connections at both ends
Coupling Rigid-Hinge	Rigid coupling with bending-resistant connection at member start and hinged connection at member end
Coupling Hinge-Hinge	Rigid coupling with hinged connections at both ends (only axial and shear forces are transmitted, but no moments)
Coupling Hinge-Rigid	Rigid coupling with bending-resistant connection at member end and hinged connection at member start
Spring	Member with spring stiffness, definable activity zones, and damping coefficients
Dashpot	Member with viscous damping properties for RF-DYNAM Pro
Null	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:

$E·A \text{and} G·I_T : \hspace{0.17em}{10}^{13}·\mathcal{l} \text{[SI unit]} \text{(}\mathcal{\text{l}}\text{=member length)}$

• Flexural resistance:

$E·I : {10}^{13}·{\mathcal{l}}^3 \text{[SI\hspace{0.17em}unit]}$

• Shear stiffness (if activated):

$G_{Ay} \text{or} G_{Az} : {10}^{16}·{\mathcal{l}}^3 \text{[SI\hspace{0.17em}unit]}$

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.

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.

$N_{cr}=\frac{{\pi }^{2}EI}{{\mathcal{l}}_{cr}^2} \text{where} {\mathcal{l}}_{cr}=\mathcal{l}$

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.

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 u_x 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 u_x 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 4.163) 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.

Stiffnesses of couplings are calculated depending on the model to preclude 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 C_1,1 describes the stiffness of the member in its local x-direction according to the following relation:

$k=\frac{E A}{\ell }$

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 u_min and u_max define the geometric activity zone of the spring. The spring acts as a rigid member (stop) for deformations outside of the specified zone.
• Force: The values N_min and N_max 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).

This member type is relevant for time history analyses in the dynamics add-on modules RF-/DYNAM Pro - Forced Vibrations and RF-/DYNAM Pro - Nonlinear Time History. You can specify the member properties in a dialog box that you can access by using the [Edit] button in the dialog box or in the table.

This linear viscous damping element corresponds to the member type "Spring" described above. In the Dashpot tab, the Viscous damping coefficient c must also be specified. The forces that are dependent on the velocity can thus be considered in the dynamics modules. With regard to viscoelasticity, the member type "Dashpot" is similar to the Kelvin-Voigt model, which consists of the damping element and an elastic spring (both connected in parallel).

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.

The internal determination of tapered cross-section values is controlled by the Taper Shape 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.

Table column N provides information on the global axis the member is parallel to or in which plane spanned by the global axes the member lies. If there is no entry, the member is in an arbitrary spatial position.

If a member is aligned parallel to the global axis Z, and therefore in vertical position, the local axis z naturally has no Z-component. In this case, the following rule applies: The local axis y is aligned parallel to the global axis Y. Then the position of the z-axis is determined by the right-hand rule (see Figure 4.170).

When a member in a continuous set of column members is not precisely in vertical position (due to minor deviations of the nodal coordinates X or Y), the axes of the member can change their orientation: RFEM classifies the position of a member that is minimally inclined as "general". If you still want to classify members in general position as vertical, select Tools → Regenerate Model in the menu (see Chapter 7.1.3).

Member rotations can be applied in two ways:

• Member rotation via angle β

Define an Angle β by which the member is rotated. If the rotation angle β is positive, the axes y and z are rotated clockwise around the longitudinal member axis x.

• Member rotation via help node

The member axis system is directed to a particular node. First, select the axis (y or z) you want affected by the help node. Accordingly, the help node defines the plane xy or the plane xz of the member. Then, enter the help node, select it graphically, or create a new one. However, the node may not lie on the straight line that is defined by the x-axis of the member.

The following example shows columns that are aligned towards the center point.

Changes of the local member axis system may affect the algebraic signs of internal forces. The following figure illustrates the general sign convention.

In these two text boxes or table columns, you can define hinges that control the transfer of internal forces on nodes. The hinge numbers refer to the entries available in Table 1.14 Member End Hinges (see Chapter 4.14).

For specific member types, entries are not possible because internal releases already exist.

In this table column or text box of the Options dialog tab (see Figure 4.161), you can assign an eccentric connection to the member. The numbers of the eccentricities refer to Table 1.15 Member Eccentricities (see Chapter 4.15). A connection type determines the eccentricities of both member start and member end.

Member divisions control the numerical output of internal forces and deformations along the member (see Chapter 4.16). Use the settings in the table column or the text box of the Options dialog tab to assign divisions or create new ones. The numbers of the divisions refer to the entries in Table 1.16 Member Divisions.

A member division neither has any influence on the determination of extreme values nor on the graphical results diagram (RFEM internally uses a more refined partition). As member divisions are not required in most cases, the default setting is 'None' or '0'.

In this text box of the Options tab (see Figure 4.161), you can assign an elastic foundation to the member. The numbers of the elastic foundations are managed in Table 1.19 Member Elastic Foundations (see Chapter 4.19).

This text box in the Options dialog tab (see Figure 4.161) makes it possible to provide the member with nonlinear properties. The numbers of the nonlinearities refer to the entries in Table 1.20 Member Nonlinearities (see Chapter 4.20).

If different cross-sections are defined for the member start and member end, this table column or text box in the Options tab provides a choice between a Linear and a Quadratic taper application. This allows you to describe the taper geometry for the determination of the interpolated cross-section values.

In most cases, there is a linear taper course: The height of the cross-section changes evenly from the start of the cross-section to its end; the width remains more or less constant. However, if the width of the cross-section also changes distinctly along the member (e.g. taper made of solid sections), it is recommended to use a square function for the interpolation of cross-section values.

This table column states the absolute length of the member as the distance between start and end node. Eccentricities are taken into account.

You can also read the member length in the work window: Place the mouse pointer on a member and wait a moment until the ScreenTip of the member appears.

The mass of a member is determined from the product of the cross-sectional area A and the specific weight of the material. RFEM applies g = 10 m/s² as the gravitational acceleration. If necessary, you can adjust this value in the Options tab of the General Data dialog box (see Figure 12.32).

Table column N provides information about the global axis parallel to the member, or in which plane spanned by the global axes the member lies. If there is no entry, the member is in an arbitrary spatial position.

If continuous members do not have a uniform member position, problems may arise, for example, when applying aligned imperfections. The following FAQ provides an example including a solution:
https://www.dlubal.com/en-US/support-and-learning/support/faq/000619

The Effective Lengths dialog tab manages the Effective Length Factors k_cr,y and k_cr,z.

The effective length factors can be adjusted separately for both member axes. The dialog fields on the right show the Effective Lengths that result from the entered factors and the member length.

Effective length factors are significant for add-on modules such as RF-STEEL EC3 where stability analyses are performed, but they play a secondary role for RFEM, because buckling lengths for buckling members, for example, are determined internally from the boundary conditions and taken into account accordingly.

The Critical Buckling Load dialog section allows you to specify if the flexural buckling load of the member is checked during the calculation. By default, the check box is selected for truss, compression, and buckling members. The Global Calculation Parameters dialog tab of the Calculation Parameters dialog box (see Figure 7.27) provides a global setting option for this kind of control.

With the Modify Stiffness dialog tab, you can influence member stiffnesses.

You can select the Definition Type of the stiffness adjustment from the list. If you select None (no modification of stiffness), all stiffness components with the factor 1.00 are taken into account for the calculation.

Use the Multiplier Factors option to customize the stiffness factors k for torsional, bending, axial, and shear stiffnesses of the member (see Figure 4.174).

When you select the According to AISC 360-10 C2.3(2) definition type, there are different options in the dialog tab, which are in alignment with the American Steel Standard.

When determining internal forces according to ANSI/AISC 360-10, you have to consider a reduction factor τ_β for all members whose bending stiffnesses contribute to the stiffness of the structure. This factor is dependent on the member's axial force: The larger the axial force, the larger τ_β is as well.

If τ_β is to be determined Iteratively, you have to specify the Design Method – LRFD or ASD. The factor is calculated according to equation (C2-2a) or (C2-2b) of AISC 360-10 in several steps until a convergence is reached.

Independent of the factor τ_β, the reduction factor 0.8 is applied for all members for the bending and axial stiffnesses, as required in AISC 360-10. Use the Set to 1 check box to avoid the iterative determination of τ_β so that only a stiffness reduction of 0.8 is applied.

The definition type According to ACI 318-14 Table 6.6.3.1.1(a) shows the reduction factors according to the American reinforced concrete standard depending on the component type. The list provides different options to select the corresponding factors for columns or beams, for example.

Generally, overlapping members in the model are not desired. If you define a new member on the nodes of an existing member, RFEM automatically deletes the old member.