The Main tab manages the basic member parameters. If you select a check box in the 'Options' section, another dialog tab is usually added. There, you can define the details in each case.
Member Type
The member type controls how internal forces can be absorbed or which properties are assumed for the member. Various member types are available for selection in the list.
Beam Member
A beam is a bending-resistant member that can transfer all internal forces. A beam member has no hinges at its member ends. This member type can be loaded by all load types.
Rigid Member
A rigid member couples the displacements of two nodes by a rigid connection. In principle, it therefore corresponds to a Coupling. This allows you to define members with very high stiffness under consideration of hinges, which can also have spring constants and nonlinearities. Numerical problems hardly occur because the stiffnesses are adapted to the system.
For rigid members, internal forces are output if you activate the Results for Couplings in the Navigator - Results below in the 'Members' category.
The following stiffnesses are applied for rigid members:
| Axial stiffness E · A | 1013 · ℓ [SI unit] with ℓ = member length |
| Torsional stiffness G · IT | 1013 · ℓ [SI unit] |
| Flexural stiffness E · I | 1013 · ℓ3 [SI unit] |
| Shear stiffness GAy / GAz (if activated) | 1016 · ℓ3 [SI unit] |
Rib Member
Ribs can be used to represent T-beams (downstand beams). With this member type, the eccentricities and effective plate widths are considered in the FEM model.
Ribs are primarily suitable for reinforced concrete members because the rib internal forces and cross-sections are incorporated into the concrete design. A steel plate with a welded-on "rib" should be modeled as a surface with an eccentrically connected member.
The list provides several selection options for the 'Rib alignment'.
A rib is usually an eccentrically arranged member. The eccentricity is determined automatically from half the surface thickness and half the member depth. However, it can also be defined manually. The eccentricity of the rib increases the stiffness of the model. For a centric arrangement, the centroidal axis of the rib lies in the middle of the surface.
The effective widths of the rib are to be defined in the 'Flange dimensions' section for the left and right side. In most cases, the 'Find automatically' setting can be kept, with which the program determines the two surfaces. If more than two surfaces meet at the line of the rib member, the governing surfaces must be defined manually.
There are various options for entering the integration widths b-y,int and b+y,int (see image New Rib): The widths can be entered directly or determined automatically from the member length using the options Lref / 6 and Lref / 8. They can also be determined according to the specifications of a standard, for example according to 'EC2' Section 5.3.2.1.
The by,int values define the width of the surface or the integration area from which the internal forces are to be integrated. The by,eff values represent the cross-section width of the rib flange from the web center to the respective edge. By default, by,int and by,eff are set equally. However, after clicking the
button, you can define them separately.
If nodes of the 'Nodes on Member' type have been defined, the rib can be defined segment-wise for the individual segments. If several segments are defined, the staggered width ranges can be connected linearly to each other via the 'Linear distribution' table column to prevent large stiffness jumps in the rib member.
For 3D models, the effective widths have no influence on the stiffness because the increased stiffness is considered by the eccentric member. However, the effective widths affect the distribution of the member and surface internal forces.
Truss Member
A truss member corresponds to a beam member with moment hinges at both ends. Additionally, the rotation about the longitudinal axis at the member start is released by a hinge φx. For this member type, bending and torsional moments from the member loads are output.
Truss Member (N only)
This type of truss member with the stiffness E ⋅ A is able to absorb axial forces in the form of tension and compression. Only node internal forces are output. The member shows a linear internal force distribution, provided no concentrated load acts on the member. No moment distribution that could occur due to self-weight or a line load is output. However, the nodal forces are calculated from the member loads, thus ensuring correct transfer.
Buckling-Restrained Brace
The Buckling-restrained brace type allows the modeling of a member with a steel core (flat steel or cruciform cross-section) and a concrete-filled casing in a square or round hollow section. It is used especially in the USA for stiffening buildings prone to earthquakes.
The steel core is movable in the concrete casing without bond. Under compression, "micro-buckling" with high eigenmodes occurs because the casing prevents global buckling of the whole member.
Only the steel core is considered for the stiffness of the member, and for the automatic self-weight, the concrete casing with the outer steel shell is also considered.
Tension Member
A tension member can only absorb tensile forces. The member type corresponds to a 'Truss Member (N only)' that fails under a compressive force.
The calculation of a framework with tension members is carried out iteratively: In the first step, the internal forces of all members are determined. If tension members receive a negative axial force (compression), another iteration step starts. The stiffness components of these members are no longer considered – they have failed. This process is continued until no more tension members fail. A system can become unstable due to the failure of tension members.
Compression Member
A compression member can only absorb compressive forces. The member type corresponds to a 'Truss Member (N only)' that fails under a tensile force. Failing compression members can lead to an unstable system.
Buckling Member
A buckling member corresponds to a 'Truss Member (N only)' that absorbs tensile forces without limit, but compressive forces only up to reaching the critical force. For Euler case 2, this force is determined as follows:
With this member type, instabilities that arise from the buckling of truss members in a nonlinear calculation according to second-order or large deformation analysis can often be avoided. If these are replaced (realistically) by buckling members, the critical load is increased in many cases.
Cable Member
A cable can only be subjected to tension. This allows you to analyze cable chains by an iterative calculation according to large deformation analysis, considering longitudinal and transverse forces.
Cables are suitable for models where large deformations with corresponding changes in internal forces can occur. For simple bracing, such as for a canopy, tension members are completely sufficient.
Reinforcement Bar
This member type allows you to model slack steel reinforcements in the FE model of a reinforced concrete element. For example, discontinuity regions based on the strut-and-tie model (tension and compression strut for corbels, beams with openings) can be investigated.
The reinforcement bar has an automatic connection function to other elements such as members or surfaces when it is physically inside the element. Like the Truss Member (N only), a reinforcement bar only has tangential stiffness. Nonlinear material behavior is not yet possible.
In the 'Settings' section, slack reinforcement is set as the member type. Further reinforcement bar types are available if the add-on Tendons is activated.
In the 'Master objects' section, assign the members or surfaces in which the reinforcement bar lies. Use the
button for this. With the
button, you can then automatically connect the reinforcement bar to the master object.
Cable on Pulleys
This cable member type also absorbs only tensile forces and is calculated according to cable theory (large deformation analysis). However, a cable on pulleys can only be defined on a polyline that has at least three nodes. Therefore, this member type is suitable for flexible tension elements whose longitudinal forces are guided through the model via deflection points. An application example is a pulley block.
In contrast to a normal cable member, only a displacement in the inner nodes in the longitudinal direction (ux) is possible. Therefore, the member must not be loaded by member loads acting in the local y- or z-direction. Only displacements ux and axial forces N are considered.
For the inner nodes of the polyline, it does not matter whether a nodal support is present or whether the member is connected to another construction: The complete system of the cable member is analyzed over the length of the polyline.
Result Beam
The result beam is suitable for integrating surface, solid, or member results in a fictitious member. This allows, for example, reading the resulting shear forces of a surface for the masonry design.
The line of a result beam can be placed anywhere in the model. The result beam requires neither a support nor a connection to the model. However, a cross-section must be assigned to enable a design. No loads can be applied to a result beam.
Select the type of the result beam in the 'Integrate stresses and forces' section to define the geometric shape of the integration area. In the 'Parameters' section, you can then define the dimensions. They are related to the line of the member at its centroid.
In the 'Include Objects' section, specify the surfaces, surface cells, solids, and members whose results should be considered in the integration. Alternatively, select 'All' objects and then exclude specific elements in the 'Excluded from inclusive objects' section.
Result Line
The result line is suitable for integrating surface, solid, or member results in a line. This line can be placed anywhere in the model.
The principle corresponds to a Result Beam. However, you do not need to assign a cross-section. In the 'Cross-section' tab, you can read the length of the line and, if necessary, rotate the line for the result display; it has no further function.
Load Transfer
This member type allows you to apply loads to objects that are connected to the member at end or intermediate nodes. The member itself has no stiffness. You can define the criteria for load transfer in a new tab.
The load transfer is currently carried out using the strip method. The loading of the load transfer member – member load or nodal load of the type force, moment, or mass – is transferred proportionally to the nearest common structural objects. These are, for example, supported nodes, members, nodes of surfaces, or supported lines.
If the self-weight of the member should be considered, you can define the member weight in the 'Parameters' section.
In the 'Loaded Objects' section, the numbers of the nodes at which the member load is transferred to the adjacent objects are specified. If not all of these nodes are relevant, you can exclude specific nodes in the 'Without effect on' section.
Virtual Joist
This member type allows you to use the cross-section properties for Open Web Steel Joists, which the Steel Joist Institute has filed in so-called "Virtual Joist" tables. These Virtual Joist profiles represent equivalent wide-flange beams that come very close to the chord area, the effective moment of inertia, and the weight. The joist is thus replaced by a member with a virtual cross-section. In this way, complex support units, such as a truss girder, can be simulated in the overall system.
Select the 'Series' of the virtual joist in the list.
You can then specify the exact type in the 'Virtual Joist' list.
The
button in the 'Cross-section and Material' section allows you to import the virtual joist from the cross-section library.
Surface Model
This member type is primarily suitable for modeling cellular and castellated beams or cross-section weaknesses, such as openings for supply lines, in the member model. The member is converted into a surface model in which the Member Openings are arranged according to user specification. However, the member itself is preserved. The following conditions must be met:
- The cross-section represents a standardized or parameterized thin-walled profile with a web.
- The material of the cross-section is based on an isotropic linear-elastic material model.
With the 'Surface model' member type, the member exists as both a member object and a surface object. The geometric properties are identical; both models have the same centroid. The display is controlled in the Navigator - Display via the entry Model → Base Objects → Members → Surface Model or the
button in the toolbar.
The FE mesh of the surface model is generated automatically and cannot currently be influenced. The surface model is used for the static calculation. For evaluation, both the member results are available (as with a Result Beam, where the stresses of the member partial surfaces are integrated into member internal forces) and the surface results. Here, too, control can be made via the Navigator - Display or the
button.
The design of a surface model member in the add-ons is carried out using the member internal forces and the member cross-section.
As can be seen in the image above, several Rigid Members are created at the member ends of a surface model member. They connect the surface model to the end nodes of the adjacent members. This ensures the correct transfer of internal forces to the 1D objects. If several surface model members adjoin each other, these coupling members are created for each member.
In this case, define a Force Eccentricity at the cross-section for the member load. The load is thus applied realistically at the cross-section edge and is preserved in the surface model.
Stiffness
With this member type, you can use a member with user-defined stiffnesses. The stiffness parameters must be defined in the 'New Member Stiffness' dialog (see chapter Member Stiffnesses).
Coupling
A coupling member is a virtual, very stiff member with rigid or hinged member ends. There are four options to couple the degrees of freedom of the start and end nodes 'Fixed' or via a 'Hinge'. Couplings allow you to model special situations for force and moment transfer. The axial and shear forces or torsional and bending moments are transferred directly from node to node.
Spring
A spring member offers the possibility of modeling linear or also nonlinear spring properties with definable effective ranges. For a spring member, you only need to define the member length Lz in the 'Cross-section' tab, not a cross-section: The stiffness of the member results from the spring parameters that you define in the 'New Member Spring' dialog (see chapter Member Springs).
Damper
A damper corresponds in principle to a spring member with the additional property 'Damping coefficient'. This member type extends the possibilities for dynamic analyses according to the Time History Analysis.
As with a spring member, you only need to define the member length Lz in the 'Cross-Section' tab, not a cross-section. The stiffness of the member results from the spring parameters that you define in the 'New Member Spring' dialog (see chapter Member Springs). You can control the damping properties via the damping coefficient X.
Options
In this section, you can define further member properties via the check boxes.
Nodes on Member
With one or more nodes on the member, you can divide the member into segments without dividing the member (see chapter Nodes).
Hinges
You can arrange hinges on a member to control the transfer of internal forces at the end nodes (see chapter Member End Hinges). Input is locked for specific member types because internal hinges already exist. You can assign hinges to the 'Member start i' and the 'Member end j' separately.
Eccentricities
Eccentricities offer the possibility of connecting the member eccentrically at the end nodes (see chapter Member Eccentricities). You can assign eccentricities to the 'Member start i' and the 'Member end j' separately.
Supports
You can assign a support to the member that is effective over its entire length. The degrees of freedom and spring stiffnesses must be defined in the support conditions (see chapter Member Supports).
Transverse Stiffeners
Transverse stiffeners on the member have an influence on the warping stiffness of the member. They affect the calculation with warping torsion considering seven degrees of freedom (see chapter Member Transverse Stiffeners).
Member Openings
Member openings affect the cross-section values and the internal force distribution. They are relevant for the 'Surface model' member type. Chapter Member Openings describes how you can define the type and the position of the openings.
Nonlinearity
You can assign a nonlinearity to the member. The nonlinear properties must be defined as member nonlinearities (see chapter Member Nonlinearities).
Result Intermediate Points
With result intermediate points, you can control the table output of the results along the member. The division points must be defined in the 'New Member Result Intermediate Point' dialog (see chapter Member Result Intermediate Points).
End Modifications
With end modifications, you can graphically adjust the geometry of the member at its ends. This allows you to prepare overhangs, shortenings, or bevels for the rendered display.
'Extension': You can define an 'Extension' for the member start and the member end. A negative value Δ acts as a shortening.
'Slope': With a slope, you can bevel each member end. Inclination angles about the two member axes y and z are possible. A positive angle causes a clockwise rotation about the respective positive axis.
Activate Load Transfer
The check box enables you to distribute the loading of the member – regardless of the member stiffness – using a load transfer. Thus, the member is effective in the model through its stiffness. The distribution of the load to the neighboring objects, however, is controlled via the parameters that you can define in the Load Transfer tab.
Deactivate for Calculation
If you select this check box, the member, including its loading, is not considered in the calculation. This way, you can investigate how the structural behavior of the model changes when certain members are not effective. The members do not need to be deleted; the loads are also retained.
