5.1                       General Criteria

Three fundamental types of entities can be checked or designed: beams, shells (concrete) and solid sections. Properties of these entities are grouped into the following concepts:

Beam and Shell Properties: associated with beam and shell elements. It is the parallel concept to real constants and sections of ANSYS. It contains all the element properties necessary for the calculation of the model and postprocessing with CivilFEM.

Solid Sections: associated to elements of a 3D model of finite elements. It contains all the properties necessary for the postprocessing of the cross sections with CivilFEM. It extends the checking capacities to two-dimensional and three-dimensional solid models.

Therefore, beam and shell properties associated to beam elements will contain the following:

-          Dorsal cross-section (I)

-          Frontal cross-section (J)

-          Member properties

-          Other parameters (offsets, etc.)

If beam and shell properties are associated to shell elements, the information will consist of:

-          Shell vertex in I node

-          Shell vertex in J node

-          Shell vertex in K node

-          Shell vertex in L node

-          Member properties

-          Other parameters (EFS, etc.)

With respect to solid sections captured from a finite element model, the information will include:

-          Cross section

-          Member properties

The above concepts are briefly explained in more detail hereafter:

 

A.1 Cross Section: This concept refers to a unique cross section, as commonly understood in engineering.

A.2 Shell Vertex: refers to the data of a shell vertex. It is a concept parallel to the cross section and is used to represent properties of a particular vertex of the shell element.

B.    Member properties: These properties include parameters related to codes, but not related to the cross section. It refers to the member itself without including the ends.

A detailed description of each one of these concepts and of the different groups of properties necessary for the definition of sections in CivilFEM is explained in the following sections.

 

5.2                       Cross Sections

Cross sections in CivilFEM, as previously stated, refer to a unique cross section. It does not coincide with the concept of Group of Real Constants of ANSYS which includes the data for both sections (I, J) of a beam element. Each beam element will have associated two cross sections that will correspond to both ends.

5.2.1                      General Properties

General properties are those properties common to all cross sections. These properties have the following labels and values:

Rf16	Identification of cross section (maximum of 16 characters). For hot rolled steel shapes it contains the library reference, and for other sections it holds a label dependent on STP: STP=0: Rf16= Generic STP=1: Rf16= Structural Steel STP=2: Rf16= Reinforced Concrete STP=3: Rf16= Concrete + Steel
Name	Name assigned to the cross section (maximum of 32 characters).
Stp	Type of transversal cross section: 0 Generic 1 Structural Steel 2 Reinforced Concrete 3 Concrete + Steel
Shp	Section Typology 0 Generic 1 I Section 2 Channel 3 Pipe 4 Angular 5 Square/Rectangular 6 Box 7 Circular 8 Simple T
Csys	Number of the section’s coordinate system. Once the section is defined, the number of the local system is stored; however, the data referring to new coordinates are not updated.
Coor	X, Y, Z origin location of the section’s coordinate system according to the global coordinate system.
Angl	THXY, THYZ, THZX rotation angles in degrees of the section’s coordinate system according to the global coordinate system.
Mcos	Cost of materials per unit length.
Scos	Additional cost per surface unit.
Lcos	Additional cost per unit length
Perm	Perimeter of the section.
Tcos	Total cost per unit length. The stored value is the summation of (MCOS+SCOS*PERM+LCOS).

5.2.2                      Dimensions

These measurements only apply to sections defined by dimensions or defined from the library. The definition of each variable depends on a particular section. Labels referring to welded and hot rolled steel sections (see commands ~SSECDMS and ~SSECLIB) are:

H	Total depth of the section
Tw	Web thickness
B	Total width of the section
Tf	Flange thickness
Hi	Web height between the inner faces of the flanges.
A/r1	Weld throat thickness/ Fillet radius on the union between flange and web
R2	Fillet radius on the edge of the flange
D	Web free depth between welding chords

Every concrete section has particular geometric properties. The geometric properties of an I-section are shown below:

 

Geometric Properties of Concrete Sections

where:

 

Depth	Total depth
Tw	Web thickness
BfTop	Width of top flange
TfTop	Thickness of top flange
BfBot	Width of bottom flange
TfBot	Thickness of bottom flange

The geometric properties of concrete cross sections that can be defined with CivilFEM are shown with the ~CSECDMS command.

5.2.3                      Points and Tessella

The cross sections in CivilFEM are made of points and tessella. Points support the geometric description of the cross section and the tessella support the geometric resistance. All resisting properties are exclusively calculated from the tessella structure of the section, except for sections from the library whose values are obtained directly from the hot rolled shapes manual.

Points and tessella do not have user-numbering capabilities; CivilFEM numbers them internally and consecutively. The user may control the section’s mesh density by applying the command ~TREFINE. This command doubles the number of divisions; therefore, the number of tessella is multiplied by two and the number of surfaces by four each time the command is applied.

The points that form the tessella structure are the union elements between them. Therefore, the points are common between adjacent tessella when they are formed by the same material. Nevertheless, points will be doubled if each of the adjacent tessella present different materials.

Labels and values corresponding to points are the following:

Mat	Point material number.
Mtp	Point material type: 0 Generic 1 Structural Steel 2 Concrete 3 Reinforced Steel 4 Prestressing Steel
Nod	Number of node associated to the point. It will be 0 if there are no associated nodes.

 

The interpolation of geometry and stresses and the integration of forces in cross sections are made through the shape of the tessella as a function of its type number and number of points. The features for each of the seven types of tessella are shown in the following table:

 

 

The labels and values corresponding to the tessella are the following:

Mat	Number of tessella material.
Mtp	Tessella material type: 0 Generic 1 Structural Steel 2 Concrete 3 Reinforcing Steel 4 Prestressing Steel
Typ	Type of tessella as indicated in the previous table.
Tpt	Points that contain the tessella.
Elm	Number of the element associated to the tessella. If there is not an associated element, its value will be 0.
Efn	Number of the section’s face or node associated to the tessella. Its value will be 0 if the tessella is not associated with any face or node.
Rnf	Number of the flexural reinforcement group associated to the tessella. Its value will be 0 if the tessella is not associated to any reinforcement group.
Plt	Number of the plate associated to the tessella. Its value will be 0 if the tessella is not associated to a plate.
Geo	Additional tessella geometric data. Possible values depend on the type of tessella. For tessella points (type 1): Corresponds to the tessella area. For linear tessella (types 2 and 3): Corresponds to the thickness of the tessella on its i and j ends.

 

5.2.4                      Plates

All steel sections (hot rolled or by dimensions) in CivilFEM are made of a plate structure, whose properties are automatically defined by the program. However, if a section is defined by the user by plates (see command ~SSECPLT), then the plate properties must also be identified by the user.

The plate structure describes the section as a group of independent plates (webs or flanges) in order to check elements with Eurocode No.3. For each plate, the following data is defined:

Mat	Number of the material associated to the plate.
Mtp	Plate material type: 0 Generic 1 Structural Steel
Pty	Plate type for bending moment MY. 0 Not defined 1 Flange 2 Web
Ptz	Plate type for bending moment MZ. 0 Not defined 1 Flange 2 Web
Cp1	Union condition for the end point 1 of the plate. 0 Free 1 Fixed
Cp2	Union condition for the end point 2 of the plate. 0 Free 1 Fixed
Esp	Plate thickness
Yp1	Y coordinate of end point 1
Zp1	Z coordinate of end point 1
Yp2	Y coordinate of end point 2
Zp2	Z coordinate of end point 2

To modify these data see commands ~SECMDF and ~SSECPLT.

5.2.5                      Faces

Faces in CivilFEM support the definition of the bending reinforcement. Each face consists of a succession of segments located on the section points. Faces can be defined on any point of the section, thus allowing the free localization of bending reinforcement groups. The numeration determines the side on which the reinforcement is positioned with the following approach:

 

 

Properties referring to faces are:

 

Npt	Number of points that belong to the face.
Upt	Point numbers.

To erase, define or modify the faces of a cross section, see ~SECMDF command.

5.2.6                      Reinforcement Definition

CivilFEM supports the definition of bending, shear and torsion reinforcement (see ~RNFDEF and ~RNFMDF commands). Data corresponding to each of these three types of reinforcements are described next.

 

5.2.6.1                  Bending Reinforcement

The bending reinforcement of the concrete sections is organized into groups with no limit on the quantity of groups defined.

The reinforcement groups can be located on any face defined in the section. Bending reinforcement groups in CivilFEM can be defined with the one of the following:

Ast	Total reinforcement group area
Asl	Reinforcement group area per unit length
N-Fi	Number of bars in a group and its diameter
NL-Fi	Number of bars in a group per unit length and its diameter
S-Fi	Space between bars and diameter of bars

When the bending reinforcement is introduced by any of the five options above, the rest of the data will calculated automatically. If reinforcement is defined by bars, specifically, not distributed uniformly, and the number of bars is not an integer, CivilFEM will round this number to the closest natural number and recalculate the new corresponding space among the bars.

The preliminary reinforcement amount and initial distribution (automatically defined by the program) can be defined using the RKEY parameter. Different RKEY’s exist for each concrete section type defined in CivilFEM (see command ~CSECDMS).

Data referring to this group are:

 

Rkey	Initial reinforcement label (see ~CSECDMS command for the different RKEY values depending on the type of section).
Rmat	Material number of the reinforcement groups defined by initial reinforcement. (RKEY>0).
Urf	User reinforcement group number.
Mat	Material number associated to the reinforcement group (used when RKEY=0).
Cls	Class of the reinforcement group. 0 Scalable reinforcement (the amount of the reinforcement can be increased or reduced by CivilFEM in the design process). 1 Fixed reinforcement (the reinforcement amount will not be modified by CivilFEM in the design process)
Fi	Reinforcement group bars diameter.
Ufc	Face number associated to the reinforcement group.
End	Situation of the reinforcement group bars at the ends of the face: 0 Includes bars at both ends of the face.

 

 

The bar spacing is calculated by the following expression:

S = L / (N -1)

 

1	Include bar only at end 1.

 

 

The bar spacing is calculated by the following expression:

S = 2*L / (2*N -1)

 

2	Include bar only at end 2.

 

 

The bar spacing is calculated by the following expression:

S = 2*L / (2*N -1)

3	Do not include bars at both ends. This value should be used for circular sections to avoid bars superposition at both ends.

 

 

The bar spacing is calculated by the following expression:

S = L/ N

 

4	Include bars at both ends with a distance equal to the mechanical cover (Mc).

 

 

The bar spacing is calculated by the following expression:

S = (L-2*Mc)/(N-1)

 

Mc	Mechanical cover.
Gc	Geometrical cover: concrete clear cover.
Ast	Total reinforcement group area.
Asl	Reinforcement group area per unit length.
N	Number of bars.
Nl	Number of bars per unit length.
S	Distance between bars.

 

5.2.6.2                  Shear Reinforcement

Shear reinforcement in cross sections is defined by accurate parameters. In CivilFEM the possible input parameters include:

Ass	Area per unit length.
As-S	Input of a stirrups’ total area and the distance between stirrups.
N-S-Fi	Input of the longitudinal spacing of the stirrups and the diameters of bars.

Data of this group are the following:

MAT	Material number of shear reinforcement.
ALPY	Angle of the shear Y stirrups with the longitudinal axis of the member (degrees).
ALPZ	Angle of the shear Z stirrups with the longitudinal axis of the member (degrees).
ASSY	Area per unit of length for shear Y.
ASSZ	Area per unit length for shear Z.
ASY	Area of stirrups for shear Y
ASZ	Area of stirrups for shear Z
S	Longitudinal spacing of the stirrups.
FI	Diameter of stirrups’ bars (in mm).
NY	Number of legs for shear Y.
NZ	Number of legs for shear Z.

 

5.2.6.3                  Torsion Reinforcement

The possible input parameters for torsion reinforcement definition are the following:

Transverse torsion reinforcement:
AssT	Introduction of the total transverse reinforcement area per unit of length.
AsT-s	Introduction of the total area of the stirrup and distance between stirrups.
FiT-s	Introduction of the diameter of the stirrup and distance between stirrups.
Longitudinal torsion reinforcement
Asl	Introduction of the total longitudinal torsion reinforcement area.
N-FiL	Number of bars and diameter.

 

MAT	Material number associated to torsional reinforcement
ASST	Area per unit length of transversal reinforcement
AST	Stirrups area for torsion.
S	Longitudinal spacing of the stirrups
FIT	Diameter of stirrups bars.
ASL	Total area of longitudinal reinforcement.
FIL	Diameter of bars of longitudinal reinforcement.
N	Number of longitudinal bars.

5.2.7                      Mechanical Properties

CivilFEM uses mechanical properties of cross sections for the calculation of stresses inside the sections and for checks according to codes. All properties refer to the axis parallel to the section axis passing through the section’s centre of gravity.

There are eight possible versions of mechanical properties, depending on the type of section and the material, as shown herein:

1	Generic Gross Section
2	Steel Gross Section
3	Net Steel Section
4	(Not used)
5	Concrete Gross Section
6	Net Concrete Section
7	Homogenized Concrete Section
8	Equivalent Mixed Section

The different versions contain the tessella homogenized contribution with the following types of materials.

 

Section / Type of material	Structural Steel	Concrete	Reinforced Concrete	Prestressed Concrete	Others
Generic Gross Section	Yes	Yes	Yes	Yes	Yes
Steel Gross Section	Yes
Net Steel Section	Yes
Concrete Gross Section		Yes
Net Concrete Section		Yes
Transformed Concrete Section		Yes	Yes	Yes
Equivalent Composite Section	Yes	Yes	Yes	Yes

The properties of the net steel and concrete sections are the same as those of the gross section, except for the area (the area of the reinforcement of a concrete section and the area of the holes for a steel section will be subtracted according to the particular code).

For properties of concrete transformed sections, the net area is calculated by subtracting the area of the reinforcement and adding the area of the reinforcement multiplied by the ratio among modules of elasticity (n) for homogenization.

For properties of concrete equivalent composite sections, the net area calculation is the same as transformed sections; however, the area of the different materials that compose the section is multiplied by the ratio among modules of elasticity (n) and added for homogenization.

Valid labels of the homogenization properties are as follows:

 

HMAT	Material used for the homogenized section properties (by default, the lowest material number of the section).
KHOM	Mechanical properties homogenization key: 0 Not homogenized 1 Homogenized using elasticity modulus. (Default option)

For each of the sections the following properties are defined:

A	Area of the section
IXX	Torsional inertia
IYY	Y inertia moment
IZZ	Z inertia moment
WY	Y elastic modulus
WZ	Z elastic modulus
WPY	Y plastic modulus
WPZ	Z plastic modulus
IY	Radius of gyration in Y
IZ	Radius of gyration in Z
YG	Y coordinate of GC
ZG	Z coordinate of GC
YMN	Minimum Y coordinate of section outline
YMX	Maximum Y coordinate of section outline
ZMN	Minimum Z coordinate of section outline
ZMX	Maximum Z coordinate of section outline
YS	Distance from GC to Y top fiber (Y top)
ZS	Distance from GC to Z top fiber (Z top)
YM	Distance from GC to centre of shear forces M in Y
ZM	Distance from GC to centre of shear forces M in Z
IW	Modulus of torsional warping
IYZ	Inertia product
YWS	Y Shear area
ZWS	Z Shear area
XWT	Torsional modulus
IUU	U flexural inertia
IVV	V flexural inertia
IU	Radius of gyration in U
IV	Radius of gyration in V
ALP	Angle gyrated to go from Y to U-axis or from Z to V-axis (degrees)
V1	Distance from U to extreme fiber (for L sections).
V2	Distance from U to extreme fiber (for L sections).
U1	Distance from V to extreme fiber (for L sections).
U2	Distance from V to extreme fibre (for L sections).
U3	Distance from V to extreme fibre (for L sections).

 

Axes of Angular Sections (L)

5.2.7.1                  Computation of torsional inertia constant, torsional warping constant and shear center in generic sections

CivilFEM only computes torsional inertia (IXX), torsional warping constant (IW) and shear center (YM, ZM) for generic sections of a single material (homogeneous) and are of the following types:

·         Solid: discretized with tesella of types 4 to 7.

·         Open thin-walled: discretized with tesella of type 2. In this case IW, YM and ZM are not calculated and they are assigned the value zero.

·         Closed thin-walled of a single cell: discretized with tesella of type 2. In this case IW, YM and ZM are not calculated and are assigned the value zero.

In the following types of section are not computed, returning zero value, IXX, IW, YM y ZM:

·         Composite in which are combined the type of tesella 2 with types 4 through 7.

·         Composite in which are used different materials in a same type of tesella of types 2, 4 through 7.

·         Generic or steel defined by plates.

Currently CivilFEM not detect the section types shown below:

·         closed thin-walled multi-cellar,

·         thin-walled combining the open and closed types.

So in these cases the calculated values of IXX, IW, YM and ZM are incorrect.

The most general procedure to define a section is by a solid section, since some of the aforementioned limitations regarding thin-walled sections are avoided. In solid sections the procedure to obtain IXX, IW, YM y ZM follows the following reference:

M. Schulz, F.C. Filippou. Generalized Warping Torsion Formulation, Journal of Engineering Mechanics, pp. 339-347 (1998).

Below are indicated some considerations related to discretization of solid sections:

-        Linear tesella (types 4 and 6) can be combined quadratic tesella (types 5 and 7) but the results are more precise when tessella of same order of approximation are used.

-        It is convenint that the mesh of the section is as consistent as possible to calculate more accurately the properties of the section. This is especially important in composite sections created by command ~SEC2DIN inasmuch as can be generated incongruent meshes, in this case the user should do corrections to improve the mesh connectivity.

-        All parts have to be connected by at least one node, otherwise the coefficient matrix of the boundary value problem which is solved is singular. In this case zero value is assigned to IXX, IW, YM y ZM.

5.2.8                      Structural Properties

Structural properties are properties of cross sections which are used in structural analysis and transferred to ANSYS as real constants for the calculation of the model. They depend on the type of section used in the calculation (ASEC); the type may be any of the 8 different variations described in the previous section. (command ~SECMDF).

The different structural properties are described in the following data:

 

ASEC	Type of section used for the structural properties calculation. 1 Generic Gross Section. 2 Steel Gross Section. Default value for steel sections. 3 Net Steel Section. 4 (Not used). 5 Concrete Gross Section. Default value for concrete sections. 6 Net Concrete Section. 7 Transformed Concrete Section. 8 Equivalent Composite Section. Default value for composite sections.
YMN	Minimum Y coordinate of section outline.
YMX	Maximum Y coordinate of section outline.
ZMN	Minimum Z coordinate of section outline.
ZMX	Maximum Z coordinate of section outline.
TKY	Y Width.
TKZ	Z Width.
ARE	Area.
IXX	Torsional inertia.
IYY	Y inertia moment.
IZZ	Z inertia moment.
YCG	Distance from GC to Y top fiber (Y top).
ZCG	Distance from GC to Z top fiber (Z top).
YMS	Distance from GC to centre of shear forces M in Y.
ZMS	Distance from GC to centre of shear forces M in Z.
YWS	Y Shear area.
ZWS	Z Shear area.
XWT	Torsional modulus.

The material associated with each element of the ANSYS model must be the same as its section if gross or net properties are taken, or it must be the same as the homogenization material if properties chosen by structural calculation are homogenized (homogenized sections of concrete and equivalent mixed sections).

When defining sections with CivilFEM, the mechanical properties used for structural calculation correspond, by default, to gross sections (steel and concrete sections) or to homogenized sections in the case of mixed sections.

5.2.9                      Code Properties

Code properties are cross section properties associated to codes. To modify code properties see the ~SECMDF command.

These properties are explained in detail for every code within their respective chapter of code checking within this Manual.

5.2.10                  Steel Sections Data

Steel sections data are only defined for hot rolled steel sections (defined through the hot rolled shape library)

 

IDX1	CivilFEM index of the group.
IDX2	Shape index.

5.2.11                  Concrete Sections Data

For reinforced concrete sections, in addition

apart from the data referring to cross sections previously explained, CivilFEM will calculate and store the following data:

ROG	Geometric amount of flexure reinforcement.
ROM	Mass amount of flexure reinforcement.

 

5.3                       Axis Orientation in Beam Sections

CivilFEM uses two coordinate systems in beam sections: the CivilFEM axis system

(X_CF, Y_CF, Z_CF) and the section axes system (X_S, Y_S, Z_S).

 

CivilFEM uses the ANSYS beam element coordinate system convention as follows:

1.   The CivilFEM axis X_CF follows the element axis from node I to node J. The CivilFEM axis Y_CF can be defined in three different ways:

a.    Its orientation by default is parallel to the XY global plane. In the case where the element Y axis is parallel to the Z axis, CivilFEM axis Y_CF will be parallel to the Y global axis.

b.     In the case where the element is defined with three nodes I, J and K, the CivilFEM XY local plane will contain the node K. (This is the recommended approach)

c.    As an alternative to criterion a, the orientation of the CivilFEM Y_CF axis may be changed with a real constant, in which the axis angle of rotation q with respect to its position by default previously indicated in point a is specified.

d.    If both b and c are defined, the third node option takes precedence.

2.    The CivilFEM local axis forms a right-handed axis system with X_CF and Y_CF.

For the orientation of the cross sections of the shapes in the CivilFEM axis system, the center of gravity of the section coincides with the origin of these axes and the shape of the web is parallel to the CivilFEM Y axis.

Furthermore, the section axis system (X_S, Y_S, Z_S) is located on a singular point of the section’s geometry, parallel to the CivilFEM axis. This system includes the coordinates of the center of gravity, the points of the section, and the coordinates of the plate’s structure for steel sections. The location of this section axis system is conventional and depends on the type of section considered.

Another coordinate system exists for steel sections and for each particular code where the user can indicate the results they wish to obtain; these results are given in this system. These coordinates systems do not have to coincide with the ones listed above, and their location is shown in the corresponding sections of this Manual.

The following graphics show the location and the orientation, for the different sections, of both the CivilFEM axis system and the section axis system, denominated as follows:

            - X_CF    X axis of the CivilFEM axis system

            - Y_CF    Y axis of the CivilFEM axis system

            - X_S     X axis of the Section axis system

            - Y_S     Y axis of the Section axis system

Beam sections of reinforced concrete

 

Beam Steel Sections (rolled and welded)

5.4                       Shell Vertex

A shell element is defined by its three or four nodes. It provides information about its plane geometry, but cannot provide other required information, such as thickness, reinforcement amount (for concrete shells), etc.

This additional information will be provided in the Shell Vertex for each node of the element (it can be the same for all the nodes or even the same for a set of elements).

Therefore, this is equivalent to the cross section of a beam.

For the definition and modification of shell vertex properties, see commands ~SHLRNF and ~SHLMDF

The properties of this group are the following:

STP	Shell vertex type 0 Generic 1 Reinforced Concrete
THK	Thickness of shell vertex
MAT	Material number of the shell vertex.
MTP	Material type of the shell vertex: 0 Generic. 1 Concrete.

The data of shell vertex reinforcement are as follows:

MAT	Material of the shell vertex reinforcement.
MC	Mechanic cover of the reinforcement (same value for all)
MCXT	Mechanic cover of the reinforcement at X Top.
MCXB	Mechanic cover of the reinforcement at X Bottom
MCYT	Mechanic cover of the reinforcement at Y Top
MCYB	Mechanic cover of the reinforcement at Y Bottom
ASSXT	Reinforcement area per unit length at X Top.
ASSXB	Reinforcement area per unit length at X Bottom.
ASSYT	Reinforcement area per unit length at Y Top.
ASSYB	Reinforcement area per unit length at Y Bottom.
SXT	Separation between bars in X top face
SXB	Separation between bars in X bottom face
SYT	Separation between bars in Y top face
SYB	Separation between bars in Y bottom face
PHIXT	Diameter of X top bars
PHIXB	Diameter of X bottom bars
PHIYT	Diameter of Y top bars
PHIYB	Diameter of Y bottom bars
KRNF	Reinforcement condition: 0 Enclosed by stirrups. 1 Not enclosed by stirrups.
ALP	Angle of the reinforcement according to Y-axis to the element local Y axis.

 

5.5                       Member Properties

Member properties contain additional data for checking and dimensioning operations conforming to codes. These data envelope properties are not directly associated with the transverse cross section but with its function as a member or group of elements in a model (see command ~MEMBPRO for their definition).

5.5.1                      Eurocode No. 3

According to Eurocode No.3, member data necessary for element checks are as follows:

L	Length between lateral restraints.
K	Lateral buckling k factor (Annex F.1.2).
KW	Lateral buckling kw factor (Annex F.1.2).
C1	Lateral buckling C1 factor (Annex F.1.2).
C2	Lateral buckling C2 factor (Annex F.1.2).
C3	Lateral buckling C3 factor (Annex F.1.2).
BETAMY	Equivalent uniform moment factor (Art. 5.5.4).
BETAMZ	Equivalent uniform moment factor (Art. 5.5.4).
BETAMLT	Equivalent uniform moment factor (Art. 5.5.4).
PSIVEC	Reduction factor for vectorial effects (Art. 5.5.3).
LATBUCK	Member susceptible to lateral buckling? 0:Yes,1:No (Art. 5.5.4)
CFBUCKXY	Buckling factor in XY plane (Mz in CivilFEM axis).
CFBUCKXZ	Buckling factor in plane XZ (My in CivilFEM axis).
CHCKAXIS	CivilFEM axis that is “Y” axis of Eurocode No.3. 0 Not defined 1 CivilFEM “-Z” 2 CivilFEM “+Y” 3 CivilFEM “+Z” 4 CivilFEM “-Y”

5.5.2                      EA

According to EA, member data necessary for element checks are the following:

MEMBTYPE	Member type 1 Beam 2 Column
L	Unbraced length of member.
BETAXY	Buckling factor in plane XY (Mz).
BETAXZ	Buckling factor in plane XZ (My).

5.5.3                      LRFD

According to LRFD, member data necessary for element checks are the following:

L	Length between restraints (B3).
KY	Buckling factor Y axis (B7).
KZ	Buckling factor Z axis (B7).
KTOR	Length factor for torsional buckling (App.E3)
CB	Bending coefficient dependent on moment gradient (F1.2a).
LB	Lateral unbraced length (F1.2).

5.5.4                      British Standard 5950-1985

According to the British Standard 5950-1985 member data necessary for element checks are the following:

L	Length between restraints.
KLtx	Lateral torsional buckling factor K for X axis (Art.4.3.5 Table 9).
KLty	Lateral torsional buckling factor K for Y axis (Art.4.3.5 Table 9).
KCx	Coefficient for compression buckling X axis (Art.4.7.2 Table 24).
KCy	Coefficient for compression buckling Y axis (Art.4.7.2 Table 24).
CteRob	Robertson constant (Appendix C.2).
n	Slenderness correction factor (Art.4.3.7.6).
m	Equivalent uniform moment factor (Art.4.3.7.6).
DL	Depth of flange’s stiffeners (Appendix B.2.5).
CHCKAXIS	CivilFEM axis that is “X” axis of BS5950-1985. 0 Not defined 1 CivilFEM “-Z” 2 CivilFEM “+Y” 3 CivilFEM “+Z” 4 CivilFEM “-Y”

5.5.5                      British Standard 5950-2001

According to British Standard 5950-2001 member data necessary for elements checking are the following:

L	Length between restraints.
KLtx	Lateral torsional buckling factor K for X axis (Art.4.3.5 Table 13).
KLty	Lateral torsional buckling factor K for Y axis (Art.4.3.5 Table 13).
KCx	Coefficient for compression buckling X axis (Art.4.7.3 Table 22).
KCy	Coefficient for compression buckling Y axis (Art.4.7.3 Table 22).
CteRob	Robertson constant (Appendix C.2).
DL	Depth of flange’s stiffeners (Art. 4.3.6.7).
CHCKAXIS	CivilFEM axis that is “X” axis of BS5950-2001. 0 Not defined 1 CivilFEM “-Z” 2 CivilFEM “+Y” 3 CivilFEM “+Z” 4 CivilFEM “-Y”
D/a	Intermediate stiffeners depth.
mx	Equivalent uniform moment factor for major axis flexural bending (Art.4.8.3.4 Table 26).
my	Equivalent uniform moment factor for minor axis flexural bending (Art.4.8.3.4 Table 26).
mlt	Equivalent uniform moment factor for lateral torsional buckling (Arts.4.3.6.6. and 4.8.3.4 Table 18).

5.5.6                      Chinese Concrete Code GB50010

According to the Chinese code GB50010, member data necessary for element checkis are the following:

MEMBTYPE	Member type 1 Beam 2 Column 3 Bracing column for frame-wall structures 4 Wall 5 Link beam of walls
MEMBLOAD	Load type: 1 FORCE. The effect of concentrated force exceeds 75% in independent beam 2 FRAME. The member comes from frame structure 0 OTHER. Not “Frame” or “Force”

5.5.7                      Member Behavior

To control the concrete member calculation process in a linear or non-linear process, the underneath parameter must be defined. The member’s non-linear calculation option is only possible with the Bridge and Civil Non-Linearities module, whose calculation process is described in the documentation referring to the aforesaid modulus.

 

KEYNL

Member behavior: 0 Linear. Value by default. In this case, member will be calculated according to the linear elastic process. 1 Non-linear.

 

 

5.6                       Beam and Shell Properties

The Beam and Shell properties contain all the properties of a beam or shell element type not determined by their type, material or location of nodes. Once the cross sections (for beam elements) or the shell vertices (for shell elements) are defined, the definition of the beam and shell properties will associate them to the ends of the elements together with the corresponding property at member level.

This concept is parallel to the real constants and sections of ANSYS since it includes the data of both sections of a beam element and vertices of a shell element. When defining a beam and shell property, the group of real constants or ANSYS sections are automatically defined in ANSYS with the same identification number. Therefore, during this definition, it is necessary to indicate which element type will be associated with the beam and shell property so that the real constants can be correctly defined (see section 5.6.4).

5.6.1                      Beams

For beam elements, a beam and shell property will contain the following:

BEAM AND SHELL PROPERTY =  CROSS SECTION (I) + CROSS SECTION (J) + MEMBER PROPERTY + OFFSETS

5.6.2                      Shells

For shells, a beam and shell property will contain the following:

BEAM AND SHELL PROPERTY = SHELL VERTEX (I) +SHELL VERTEX (J) + SHELL VERTEX (K) + SHELL VERTEX (L) + MEMBER PROPERTY + EFS

5.6.3                      Properties

Labels referring to beam and shell properties are the following:

RF16	Beam and shell property reference (maximum 16 characters).
NAME	Name assigned to the beam and shell property (maximum 32 characters).
TYP	Beam and shell property type: 1 Beam 2 Shell
NSEC	Number of cross sections (if TYP=1) or shell vertices (if TYP=2) which compose the beam and shell property.
USEC	Number of cross sections or shell vertex which conform the (I,J,K,L) vertex of beam’s and shell’s properties
KEYOFF	Cross sections OFFSET: 0 Nodes at center of gravity. 1 Nodes at the sections coordinate system origin. 2 Location of nodes defined by the user. 3 Nodes at shear center.
ROUT	Type of element for which real constants are defined in ANSYS.
UMPR	Member property number.

 

The definition of a beam and shell property may be seen in the ~BMSHPRO command.

5.6.4                      Real Constants and Beam and Shell Properties in CivilFEM

The beam and shell properties in CivilFEM are linked to the real constant groups or sections of ANSYS in that the number identifying the beam and shell property in CivilFEM corresponds to the same number of real constant group or section (for elements BEAM188 and BEAM189) of ANSYS.

No. of CivilFEM BEAM AND SHELL PROPERTY= No. of ANSYS REAL CONSTANT

No. of CivilFEM BEAM AND SHELL PROPERTY= No. of ANSYS SECTION

The definition of a beam and shell property in CivilFEM implies the automatic definition of the group of real constants or section for the case of elements BEAM188 and BEAM189. For this definition to be performed correctly, it is necessary to indicate the element type for which the beam and shell property is defined, so that CivilFEM can place the precise data in the different element positions.

CivilFEM defines or renews the following real constants depending on the type of element used.

 

 

Real constants that correspond to optional input data and that do not directly depend on the beam and shell property definition are maintained unaltered; their values are conserved when the properties are redefining or when real constants are created with identification numbers that coincide with those that already exist.

The database of CivilFEM stores the section data necessary for CivilFEM's postprocessor in addition to the data necessary for solving the model with ANSYS. CivilFEM provides many commands to listed or modified the specified data (see commands ~SLDLST, ~SECMDF, ~SHLLST, ~CSLST). The modification of cross section data directly within the group of real constants or within the ANSYS sections will only be reflected in the calculation of the model with ANSYS and will not reinstate the beam and shell data stored in CivilFEM's database.

The relating cross section code data (see command ~SECMDF) and the reinforcement data in concrete sections (see commands ~RNFDEF and ~RNFMDF) are associated with the sections. Therefore, sections of the same type and with same geometric properties that have different code properties or reinforcement will need to be defined as different sections. A redefinition of the section does not modify the values of the code data or the values of the previous reinforcement (whenever the redefined section is the same type and shape).

Code properties depend on the active code and will therefore need to be defined for the specific code chosen for postprocessing. The definition of the code properties will only affect the active code does not eliminate the definition of these properties for other codes.

Section data is in user units.

5.6.5                      ANSYS Sections and CivilFEM Beam and Shell Properties

When defining a beam and shell property for elements BEAM188 and BEAM189, it is necessary to select a section from among the different types.

Rectangular, circular, pipe and box sections are defined using the commands (SECNUM, SECTYPE, SECDATA, SECOFFSET) when matching the CivilFEM definition data of the beam and shell properties with the data necessary to define sections in ANSYS.

The channel, double T, simple T and angular L type of sections are defined making use of the commands (SECNUM, SECTYPE, SECREAD, SECOFFSET). These are sections whose ANSYS section subtype is described in the SECTYPE command as MESH. The data of the ANSYS section are generated from the data of the definition the CivilFEM beam and shell property, which signifies that the nodes and cells of the corresponding ANSYS section are numbered automatically as indicated in the following figures:

 

U channel section

Double T section

Angular L section

 

Simple T section

For Beam188 and Beam189 elements, the cross sections should be defined by dimensions or by the library for a correct definition of the beam & shell property and the corresponding ANSYS section. The definition of cross sections by plates or the utility of exporting/importing cross sections are not valid for these element types.

The cells and nodes distribution and numbering of the ANSYS section are independent of the distribution and numbering of the tessella and points which define the cross sections in CivilFEM.

5.6.6                      Changing the Node Location in Beam Elements from CivilFEM

 

In CivilFEM it is possible to modify the position of each of the end nodes in a beam type element using the ~BMSHOFF command. By default, nodes are assumed to be located at the center of gravity of the section (KEYOFF = 0), but can also be located at the origin of the section’s coordinate system (KEYOFF = 1), at the shear center (KEYOFF = 3) or at a location specified by the user (KEYOFF = 2).

 

5.7                       Solid Sections

A solid section is a section associated with elements of 2D and 3D models of finite elements. It is used to extend the checking capabilities of the program to generic models in 2D/3D with elements LINK, BEAM, SHELL and SOLID.

To define a solid section from a 2D or 3D model, it is necessary to select the plane of nodes that defines the section’s location and the elements that contain the characteristics of the section. The definition of a solid section results in the automatic definition of the associated cross section. This cross section will be made by points associated with the selected nodes of the model and by tessellas corresponding to the selected elements of the model that share those nodes. The tessella will have the same properties as their corresponding elements (material, type…). Thus the points and tessella will be linked to the nodes and elements of the model. This union will be used for the calculation of stresses and the integration of forces and moments.

For the definition of the solid section, in addition to selecting the plane of nodes, it is necessary to define a local Cartesian coordinate system so that the nodes will be located in the Y-Z plane. This system will be the coordinate system of the associated cross section once it is captured.

The elements of one side of the node’s plane, which will provide faces for tessella, should be adequately selected so that there are no duplicated tessella within the cross section. Captured tessella are related to faces of solid elements or vertices of beam elements.

It is important to account for possible discontinuities resulting from only selecting the elements from one side of the section at a time. It is recommended to check the results obtained by considering the elements on either side of the section.

A solid section will contain the following:

SOLID SECTION = CROSS SECTION + MEMBER PROPERTY

5.7.1                      2D Models

CivilFEM supports the definition of solid sections from a 2D model containing the following two-dimensional elements: LINK1, BEAM3, PLANE42, BEAM54, PLANE82, PLANE182, PLANE183.

The 2D model, when cut, forms a line of nodes that, when captured, become sections formed by square tessella of 4 points or by punctual tessella (the lines become surface tessella and points punctual tessella).

With PLANE elements (42, 82, 182, 183) it is possible to use KEYOPT (3) to define the desired width of the corresponding cross section. By default, the captured section will have a unitary width in CivilFEM if the plane stress or the plane strain was defined or it will have the corresponding width if the plane stress with thickness was defined.

Elements that generate punctual tessella (LINK and BEAM elements) should have the real constant AREA defined.

5.7.2                      3D Models

CivilFEM supports the definition of solid sections from a 3D model containing the following three-dimensional elements: BEAM4, LINK8, LINK10, PIPE16, PIPE20, BEAM23, BEAM24, SHELL41, SHELL43, BEAM44, SOLID45, SHELL63, SOLID64, SOLID65, SOLID72, SOLID73, SOLID92, SHELL93, SOLID95, SHELL143, LINK180, SOLID185, SOLID186, SOLID187.

In 3D models, elements that generate punctual tessella (BEAM, LINK) should have the real constant AREA defined and shell elements should have real constants related to the thickness defined. If elements do not have corresponding real constants defined (areas in BEAM and LINK elements and thickness in SHELL elements), these elements are ignored when capturing the section. When the shell element is multilayered, it defines the thickness of the tessella as the real constant thickness for the first layer.

The following table organizes the element types according to their associated tessella type; the types of elements are substituted by tessella when the section is captured. The table also lists how the different types of tessella are used by the program to form captured sections. For further details on the definition of solid sections, see command ~SLDSEC.

 

Type=1	Point	Associated elements
	Used to: -       Represent reinforcements defined by bars (Fi>0). -       Associate LINK and BEAM (I, J) elements ends.	LINK 1, 8, 10 and 180 BEAM 3, 4, 16, 20, 23, 24, 44 and 54
Type=2	Line with two points	Associated elements
	Used to: -       Represent plates. -       Associate SHELL elements faces. -       Represent reinforcements distributed uniformly by straight lines (Fi=0).	SHELL 41, 43, 63, 143
Type=3	Line with three points	Associated elements
	Used to: -       Associate SHELL elements faces with edge nodes. -       Represent reinforcements distributed uniformly by curves (Fi=0).	SHELL 93
Type=4	Triangle with three points	Associated elements
	Used to: -       Associate SOLID elements faces.	SOLID 45, 64, 65, 72, 73 and 185
Type=5	Triangle with six points	Associated elements
	Used to: -       Associate SOLID element faces with edge nodes.	SOLID 95 and 186
Type=6	Quad with four points	Associated elements
	Used to: -       Associate SOLID elements faces.	SOLID 45, 64, 65, 73 and 185
Type=7	Quad with eight points	Associated elements
	Used to: -       Associate SOLID elements faces with edge nodes.	SOLID 95 and 186