Section

 

 

 

Enter section properties for line elements (Truss, Tension-only, Compression-only, Cable, Gap, Hook, Beam Element).

 

 

 

From the Main Menu select Model > Properties > Section.

 

Select Geometry > Properties > Section in the Menu tab of the Tree Menu.

 

Click Section in the Property Tool Bar.

 

 

 

 

     

Properties (Section) dialog box

 

  •  To enter new or additional section properties

 

Click in the Properties dialog box and enter the following: Enter the section properties by entry types.

 

  •  Modification of previously entered section data

 

Select the section to be modified from the list in the Section dialog box and click to modify the related data.

 

  •  Removal of previously entered section data

 

Select the section to be deleted from the list in the Section dialog box and click .

 

  •  To copy previously entered section data

 

Select the section to be copied from the list in the Section dialog box and click .

 

  •  To modify section data from an existing fn.MCB file

 

Click and select the MCB file containing the section data or specify a file name then click . [Details]

Section List
Display section data contained in the existing fn.MCB file.

Selected List
Select section data to be imported and register them in the Selected List.

Note
If a fn.MCB is selected, all the section data contained in the existing fn.MCB file are registered in the Selected List.

Numbering Type
Specify the Import mode for section numbers.

Keep ID
Import the data keeping the same section numbers.

New ID
Assign new numbers to the imported section data.

 

  •  To modify previously entered section property numbers

 

Select the section property numbers to be renumbered from the list in the Properties dialog box and modify the related data followed by clicking . [Details]

Renumbering Section Number dialog box

 

Start number
Assign a new starting number for the material to be modified.

Increment
Enter the increment for numbering material property numbers.

Change element's material number
Modify a material property number. Using this option will modify the previously defined material property number. If this option is not checked, the selected material having previously defined number will become undefined and the additional user-defined material number will be created without any assigned elements.

 

 

Section Data Dialog

 

Section ID

 

 Section number (Auto-set to the last section number +1)

 

Note

Up to 999999 Section ID's  can be assigned.

 

 

Name

 

  Section name (Sect. Name by default if not specified)

 

 

Offset

Display the section Offset currently set. Location of the Centroid of a section is set as default. Click    to specify a section Offset away from the Centroid. Use Hidden to verify the input.

[Details]

                                                             Change Offset dialog box       

 

Offset: Specify the section Offset from the location options shown in the figure below.

 

Horizontal Offset: Specify the Offset in the transverse direction. "to Extreme Fiber" assigns the offset to the outer-most point. For a specific location of Offset, select 'User"and enter the distance from the "Centroid" to the desired Offset location. Unless the Offset is "Center-Center" the Horizontal Offset can be entered as the "User" type. For a tapered (non-prismatic) section, data input for the J-end also becomes activated.

 

Vertical Offset: Specify the Offset in the vertical direction. "to Extreme Fiber" assigns the offset to the outer-most point. For a specific location of Offset, select "User" and enter the distance from "Centroid" to the desired Offset location. Unless the Offset is "Center-Center" the Vertical Offset can be entered as the "User" type. For a tapered (non-prismatic) section, data input for the J-end also becomes activated.

 

Note 1

When Offset distance is specified, a positive (+) sign applies to Center-to-outward for Centroid reference and Extreme-to-inward for Extreme Fiber reference.

 

User Offset Reference: When section offset distance is specified as the "User" type, define the reference location.

 

Centroid: Specify the offset distance relative to the centroid of the section.

 

Extreme Fiber(s): Specify the offset distance relative to Left/Right & Top/Bottom.

 

Note 2

When User type is specified, the Offset distance and direction are entered relative to Centroid irrespective of the Center option (Centroid or Center of Section). For example, specifying "Offset: Left-Center", "Center Loc.: Center of Section" and "Horizontal offset: 0.5 " User type" will result in an Offset 0.5" to the left of the Centroid.  And if the Offset option is "Left-Center" and the Center option is Center of Section the User type for Horizontal offset becomes activated and the User type for Vertical offset becomes inactivated. The Horizontal offset defined as User type here becomes the Centroid, and the Vertical offset fixed to Center becomes the "Center of Section"

 

Note 3

When FCM Wizard is used, and "Apply the Centroid of Pier Table Section Option" is selected, the node locations of the girder will be changed as follows:

Offset: Center-Top

User Offset Reference: Extreme Fiber(s)

Vertical Offset: User, Offset Distance (i & j) = Pier Table section height-Centroid of Pier Table section

 

 

 

 

Note 4 Usage tip of Section Offset

      • Internal process of section offset

         

        A beam element is defined by two nodes and a line connecting the two nodes. This line becomes a reference line representing the beam element, which usually coincides with the neutral axis of the beam element. If a section offset is assigned to a section, the neutral axis of the member shifts by the specified offset distance, and the element reference line is placed at the offset location. The reference line is used for selecting the element, assigning loads, displaying member forces, etc. The offset of the neutral axis of the member relative to the reference line in turn is reflected in analysis as shown in the figure (c) below.

         

         

         

      • Loaded location 

         

        1. Nodal Load

         

        When an offset is assigned to a section, a nodal load remains applied to the corresponding node regardless of the offset. This results in moments due to the offset to the neutral axis as shown in the case of figure b.

         

        2. Element Beam Loads

         

        Element beam load is applied to the neutral axis of the element regardless of the section offset position. In the diagram below, the element beam load is applied to the neutral axis even though the section is offset from the reference line. Therefore torsional moment from the element beam load is not induced by the offset. Note however that the element beam load is displayed on the reference line as if it is applied to the reference line, but it is actually applied to the neutral axis.

         

         

         

      • Calculation of member forces of the elements for which section offset is applied

         

        Member forces (axial force, shear force, moment & torsion) of a beam element are calculated relative to the neutral axis. This is true even when a section offset is applied. However, the member force diagrams are displayed on the reference line. This does not mean the member forces are calculated relative to the reference line.

        Member forces diagram when section offset is applied

      • Comparison between section offset and beam end offset

         

        An offset of a section can be defined using the Beam End Offset function. For a prismatic section, a Section offset is assigned to both

        i-end and j-end identically. However, Beam End Offset can assign different offsets at i-end and j-end independently. Section offset is more useful for a tapered section as opposed to Beam End Offset as shown in the figure below.

         

        In addition, Section offset and Beam End Offset cannot be assigned simultaneously. In such a case, Section offset is ignored, and Beam End Offset only becomes effective.

         

         

        Modeling of a tapered section group when a Section offset (Center-Top) is defined

 

 

: Display the Offset specified from the Change Offset dialog box in the guide diagram of Section Data window.

 

 

 

Consider Shear Deformation

 

Select whether to consider shear deformation. This option will be applicable for structural analysis, but will not affect the effective shear areas that appear by clicking .

 

 

 

Section Properties

 

Click to display the section property data. The section property data table is either calculated from the main dimensions or obtained from the DB depending on the method of data entry.  [Details]

Area: Cross sectional area

 

Asy: Effective Shear Area for shear force in the element's local y-direction

         It becomes inactive when Shear Deformation is not considered.

 

Asz: Effective Shear Area for shear force in the element's local z-direction

        It becomes inactive when Shear Deformation is not considered.

 

Ixx: Torsional Resistance about the element's local x-axis

 

Iyy: Moment of Inertia about the element's local y-direction

 

Izz: Moment of Inertia about the element's local z-direction

 

Cyp: Distance from the section's neutral axis to the extreme fiber of the element in the local (+)y-direction

 

Cym: Distance from the section's neutral axis to the extreme fiber of the element in the local (-)y-direction

 

Czp: Distance from the section's neutral axis to the extreme fiber of the element in the local (+)z-direction

 

Czm: Distance from the section's neutral axis to the extreme fiber of the element in the local (-)z-direction

 

Qyb: Shear Coefficient for the shear force applied in the element's local z-direction

 

Qzb: Shear Coefficient for the shear force applied in the element's local y-direction

 

Peri: O: Total perimeter of the section

 

Peri: I: Inside perimeter length of a hollow section

 

y1, z1: Distance from the section's neutral axis to the Location 1 (used for computing combined stress)

 

y2, z2: Distance from the section's neutral axis to the Location 2 (used for computing combined stress)

 

y3, z3: Distance from the section's neutral axis to the Location 3 (used for computing combined stress)

 

y4, z4: Distance from the section's neutral axis to the Location 4 (used for computing combined stress)

 

Zyy: Plastic Section Modulus about the element local y-direction

 

Zzz: Plastic Section Modulus about the element local z-direction

 

 

Note 1

All the above section property data except for Area and Peri are required for beam elements.

 

Note 2

The shear deformations are neglected if the effective shear areas are not specified. Cyp, Cym, Czp and Czm are used to calculate the bending stresses. Qyb and Qzb are used to calculate the shear stresses. Peri is used to calculate the Painting Area.

 

Note 3

Zyy and Zzz are used to calculate the strength for pushover analysis when Value Type Steel Section has been assigned Design > Pushover Analysis > Define Hinge Properties.

 

Note 4 Element Stiffness data

Sections can be defined by the stiffness data entries even if the section dimensions (H, B1, ... , etc.) are not entered.

 

  • Area (Cross-Sectional Area)

    The cross-sectional area of a member is used to compute axial stiffness and stress when the member is subjected to a compression or tension force. Figure 1 illustrates the calculation procedure.

     

    Cross-sectional areas could be reduced due to member openings and bolt or rivet holes for connections. midas does not consider such reductions. Therefore, if necessary, the user is required to modify the values using the option 2 above and his/her judgment.

     

     

     

     

    Area = +dA = A1 + A2  + A3

    = (300 x 15) + (573 x 10) + (320 x 12)

    = 14070

     

    <Figure 1> Example of cross-sectional area calculation

  • Effective Shear Areas (Asy, Asz)

    The effective shear areas of a member are used to formulate the shear stiffness in the y- and z-axis directions of the cross-section.

     

    If the effective shear areas are omitted, the shear deformations in the corresponding directions are neglected.

     

    When midas computes the section properties by the option 1 or 3, the corresponding shear stiffness components are automatically calculated. Figure 2 outlines the calculation methods.

     

    Asy: Effective shear area in the ECS y-axis direction

     

    Asz: Effective shear area in the ECS z-axis direction

     

     

    <Figure 2> Effective Shear Area calculations

  • Torsional Resistance (Ixx)

    Torsional resistance refers to the stiffness resisting torsional moments. It is expressed as

     

    <Eq. 1>

     

     

    where,

    Ixx: Torsional Constant

     

    T: Torsional moment or torque

     

    G: Shear Modulus of Elasticity

     

    ¥è : Angle of twist

     

    The torsional stiffness expressed in Eq. 1 must not be confused with the polar moment of inertia that determines the torsional shear stresses. However, they are identical to one another in the cases of circular or thick cylindrical sections.

     

    No general equation exists to satisfactorily calculate the torsional resistance applicable for all section types. The calculation methods widely vary for open and closed sections and thin and thick thickness sections.

     

    For calculating the torsional resistance of an open section, an approximate method is used; the section is divided into several rectangular sub-sections and then their resistances are summed into a total resistance, Ixx, calculated by the equation below.

     

    <Eq. 2>

     

     

     

    for a e b

     

    where,

    Ixx: Torsional resistance of a (rectangular) sub-section

     

    2a: Length of the longer side of a sub-section

     

    2b: Length of the shorter side of a sub-section

     

    Figure 3 illustrates the equation for calculating the torsional resistance of a thin walled, tube-shaped, closed section.

     

    <Eq. 3>

     

     

     

    where,

    A: Area enclosed by the mid-line of the tube

     

    ds: Infinitesimal length of thickness centerline at a given point

     

    t: Thickness of tube at a given point

     

    For those sections such as bridge box girders, which retain the form of thick walled tubes, the torsional stiffness can be obtained by combining the above two equations, Eq. 1 and Eq. 3.

     

     

     

     

                                          Torsional resistance:

    Shear stress at a given point:

    Thickness of tube at a given point:

     

    <Figure 3> Torsional resistance of a thin walled, tube-shaped, closed section

     

    <Figure 4> Torsional resistance of solid sections

     

    <Figure 5> Torsional resistance of thin walled, closed sections

     

    <Figure 6> Torsional resistance of thick walled, open sections

     

    <Figure 7> Torsional resistance of thin walled, open sections

     

    In practice, combined sections often exist. A combined built-up section may include both closed and open sections. In such a case, the stiffness calculation is performed for each part, and their torsional stiffnesses are summed to establish the total stiffness for the built-up section.

     

    For example, a double I-section shown in Figure 8(a) consists of a closed section in the middle and two open sections, one on each side.

  • The torsional resistance of the closed section (hatched part)

    <Eq. 4>

     

  • The torsional resistance of the open sections (unhatched parts)

    <Eq. 5>

     

  • The total resistance of the built-up section

    <Eq. 6>

     

     

    Figure 8(b) shows a built-up section made up of an I-shaped section reinforced with two web plates, forming two closed sections. In this case, the torsional resistance for the section is computed as follows:

     

    If the torsional resistance contributed by the flange tips is negligible relative to the total section, the torsional property may be calculated solely on the basis of the outer closed section (hatched section) as expressed in Eq. 7.

     

    <Eq. 7>

     

     

    If the torsional resistance of the open sections is too large to ignore, then it should be included in the total resistance.

    (a) Section consisted of closed and open sections

    (b) Section consisted of two closed sections

    <Figure 8> Torsional resistance of built-up sections

  • Area Moment of Inertia (Iyy, Izz)

    The area moment of inertia is used to compute the flexural stiffness resisting bending moments. It is calculated relative to the centroid of the section.

  • Area moment of inertia about the ECS y-axis

    <Eq. 8>

     

    -Area moment of inertia about the ECS z-axis

    <Eq. 9>

     

     

    : area

     

    : distance from the reference point to the centroid of the section element in the z-axis direction

     

    : distance from the reference point to the centroid of the section element in the y-axis direction

     

    : first moment of area relative to the reference point in the y-axis direction

     

    : first moment of area relative to the reference point in the z-axis direction

     

    <Figure 9> Example of calculating area moments of inertia

  • Area Product Moment of Inertia (Iyz)

    The area product moment of inertia is used to compute stresses for non-symmetrical sections, which is defined as follows:

     

    <Eq. 10>

     

     

    Sections that have at least one axis of symmetry produce Iyz=0. Typical symmetrical sections include I, pipe, box, channel and tee shapes, which are symmetrical about at least one of their local axes, y and z. However, for non-symmetrical sections such as angle shaped sections, where Iyz`0, the area product moment of inertia should be considered for obtaining stress components.

     

    The area product moment of inertia for an angle is calculated as shown in Figure 10.

     

     

    <Figure 10> Area product moment of inertia for an angle

     

     

    <Figure 11> Bending stress distribution of a non-symmetrical section

     

     

    The neutral axis represents an axis along which bending stress is 0 (zero). As illustrated in the right-hand side of Figure 11, the n-axis represents the neutral axis, to which the m-axis is perpendicular. Since the bending stress is zero at the neutral axis, the direction of the neutral axis can be obtained from the relation defined as

     

     

    <Eq. 11>

     

     

     

    The following represents a general equation applied to calculate the bending stress of a section:

     

    <Eq. 12>

     

     

     

    In the case of an I shaped section, Iyz=0, hence the equation can be simplified as:

     

    <Eq. 13>

     

     

     

    where,

     

    Iyy: Area moment of inertia about the ECS y-axis

     

    Izz: Area moment of inertia about the ECS z-axis

     

    Iyz: Area product moment of inertia

     

    y: Distance from the neutral axis to the location of bending stress calculation in the ECS y-axis direction

     

     

    z: Distance from the neutral axis to the location of bending stress calculation in the ECS z-axis direction

     

    My: Bending moment about the ECS y-axis

     

    Mz: Bending moment about the ECS z-axis

     

    The general expressions for calculating shear stresses in the ECS y and z-axes are:

     

    <Eq. 14>

     

     

    <Eq. 15>

     

     

     

    where,

    Vy: Shear force in the ECS y-axis direction

     

    Vz: Shear force in the ECS z-axis direction

     

    Qy: First moment of area about the ECS y-axis

     

    Qz: First moment of area about the ECS z-axis

     

    by: Thickness of the section at which a shear stress is calculated, in the direction normal to the ECS z-

    axis

     

    bz: Thickness of the section at which a shear stress is calculated, in the direction normal to the ECS y-axis

  • First Moment of Area (Qy, Qz)

    The first moment of area is used to compute the shear stress at a particular point on a section. It is defined as follows:

     

    <Eq. 16>

     

     

    <Eq. 17>

     

     

    When a section is symmetrical about at least one of the y and z-axis, the shear stresses at a particular point are:

     

    <Eq. 18>

     

     

    <Eq. 19>

     

     

    where,

    Vy: Shear force acting in the ECS y-axis direction

     

    Vz: Shear force acting in the ECS z-axis direction

     

    Iyy: Area moment of inertia about the ECS y-axis

     

    Izz: Area moment of inertia about the ECS z-axis

     

    by: Thickness of the section at the point of shear stress calculation in the ECS y-axis direction

     

    bz: Thickness of the section at the point of shear stress calculation in the ECS z-axis direction

  • Shear Factor for Shear Stress (Qyb, Qzb)

    The shear factor is used to compute the shear stress at a particular point on a section, which is obtained by dividing the first moment of area by the thickness of the section.

     

    <Eq. 20>

      

     

    <Eq. 21>

     

     

     

    <Figure 12> Example of calculating a shear factor

  • Stiffness of Composite Sections

    midas calculates the stiffness for a full composite action of structural steel and reinforced concrete. Reinforcing bars are presumed to be included in the concrete section. The composite action is transformed into equivalent section properties.

     

    The program uses the elastic moduli of the steel (Es) and concrete (Ec) defined in the SSRC79 (Structural Stability Research Council, 1979, USA) for calculating the equivalent section properties.  In addition, the Ec value is decreased by 20% in accordance with the EUROCODE 4.

     

    - Equivalent cross-sectional area

     

     

    - Equivalent effective shear area

     

     

    - Equivalent area moment of inertia

     

     

    where,

    Ast1: Area of structural steel

     

    Acon: Area of concrete

     

    Asst1: Effective shear area of structural steel

     

    Ascon: Effective shear area of concrete

     

    Ist1: Area moment of inertia of structural steel

     

    Icon: Area moment of inertia of concrete

     

    REN: Modular ratio (elasticity modular ratio of the structural steel to the concrete, Es/Ec)

     

     

    - Equivalent torsional coefficient

     

     

 

Note 5

Determining the positions of y1~4, z1~4 of a section imported from SPC [Details]

1. Divide the section into four quadrants.

 

2. Assign the positions furthermost from the centroid in each quadrant for checking stresses.

 

 

If the webs of a section are extensively sloped as in the above diagram, the points furthermost from the centroid may not be the lowest points of the section. Use caution that the stress checking positions of quadrants 3 & 4 may be selected differently from the expectation.

 

 

Section Type

 

 

Section - DB/User dialog box

 

  • [DB/User tab]

     The section data can be entered by the following 2 methods in the dialog box:

     

     1. Select a section from the DB (database) of the standard sections for a country.

     

     2. Enter the main dimensions of a standardized section shape.

     

    Section Shape List: Select a section shape (Angle, Channel, H-Section, T-Section, Box, Pipe, Double Angle, Double Channel, Solid Rectangle, Solid Round, Octagon, Solid Octagon, R-Octagon, Track, Solid Track, Half Track, Cold Formed Channel & U-Rib).

     

    User: Enter the main dimensions of a standardized section shape.

     

    H, B1, ...: Refer to the dimension information diagram in the dialog box.

     

    DB: Select a section from the DB of the standard sections for a country.

     

    AISC2K(US): American Institute of Steel Construction, 2000 US Unit : lb, in

     

    AISC2K(SI): American Institute of Steel Construction, 2000 SI Unit : kN, m, mm

     

    AISC: American Institute of Steel Construction

     

    CISC02(US): Canadian Institute of Steel Construction (US Unit : lb, in)

     

    CISC02(SI): Canadian Institute of Steel Construction (SI Unit : kN, m, mm)

     

    BS(S): British Standard

     

    Note

    BS indicates BS4-1 revised prior to 1993.

     

    BS4 - 93: British Standard / BS 4-1 : 1993

     

    DIN(S): Deutches Institut fur Normung e.v

     

    JIS2K : Japanese Industrial Standards 2000

     

    JIS: Japanese Industrial Standards

     

    KS: Korean Industrial Standards

     

    GB-YB05: Guojia Biao Zhun-Yejin Bu Biao Zhun

     

    Pacific(SI): Bentley Pacific Standards (SI Unit : kN, m, mm)

     

    IS84: Indian Standards

     

    Revision of V.7.6.1

     

    GB-YB05: Guojia Biao Zhun-Yejin Bu Biao Zhun(2005)

     

    CNS91: Taiwan Standards

     

    Sect. Name: Enter directly a DB section name or select a desired DB from the Section list. When the section name is directly entered, it must correspond to the format of the DB section names.

     

    Ex) AISC: W36x280, BS: UB 406x178x54, DIN: HD400x288

     

    Note
    When specifying Double Angle or Double Channel sections, assign the sectional shape in the list and select User. Then, select DB and Sect. Name from Get Data from Single Angle (or Channel) or directly enter the main dimensions of the section.

     

     

 

Section - Value dialog box

 

  •  [Value tab]

    The section data can be entered by the following 3 methods in the dialog box:

     

    1. Select a section from the DB (database) of the standard sections for a country.

     

    2. Enter the main dimensions of a standardized section shape.

     

    3. Import a section generated from SPC module.

     

    Section Shape List: Assign a section shape to use.

     

    Built-Up Section: Fabricated section

     

    Note
    Check in the case of a built-up section and leave it blank in the case of a rolled steel section. The data is referred to for strength verification for steel members and compiling material quantities in BOM    .

     

    Size

    H, B1, ...: Refer to the diagram denoting section dimensions in the dialog box.

     

    The structure can be analyzed only with the stiffness data even if the section dimensions are not specified.

     

    Section Properties

    The main section dimensions entered in Size are used to calculate and display the section stiffness.

     

    Area: Cross sectional area

    Asy: Effective Shear Area for shear force in the element's  local y-direction

    It becomes inactive when Shear Deformation is not considered.

     

    Asz: Effective Shear Area for shear force in the element's local z-direction

    It becomes inactive when Shear Deformation is not considered.

     

    Ixx: Torsional Resistance about the element's local x-axis

     

    Iyy: Moment of Inertia about the element's local y-direction

     

    Izz: Moment of Inertia about the element's local z-direction

     

    Cyp: Distance from the section's neutral axis to the extreme fiber of the element in the local (+)y-direction

     

    Cym: Distance from the section's neutral axis to the extreme fiber of the element in the local (-)y-direction

     

    Czp: Distance from the section's neutral axis to the extreme fiber of the element in the local (+)z-direction

     

    Czm: Distance from the section's neutral axis to the extreme fiber of the element in the local (-)z-direction

     

    Qyb: Shear Coefficient for the shear force applied in the element's local z-direction

     

    Qzb: Shear Coefficient for the shear force applied in the element's local y-direction

     

    Peri:O: Total perimeter of the section

     

    Peri:I: Inside perimeter length of a hollow section

     

    Note
    The value of Peri:I is '0' for an I-shaped section since the section is not hollow.

     

    Cent:y: Centroidal distance in ECS y-axis

     

     

    Cent:z: Centroidal distance in ECS z-axis

     

    y1, z1: Distance from the section's  neutral axis to the Location 1 (used for computing combined stress) The user may specify

    the location of the stress display.

     

    y2, z2: Distance from the section's  neutral axis to the Location 2 (used for computing combined stress) The user may specify

    the location of the stress display.

     

    y3, z3: Distance from the section's  neutral axis to the Location 3 (used for computing combined stress) The user may specify

    the location of the stress display.

     

    y4, z4: Distance from the section's  neutral axis to the Location 4 (used for computing combined stress) The user may specify

    the location of the stress display.

     

    Zyy: Plastic Section Modulus about the element local y-direction

     

    Zzz: Plastic Section Modulus about the element local z-direction

     

     

 

Section - SRC dialog box

 

  •  [SRC tab]

    Enter the section property data for steel RC composite members in the dialog box.

     

    Shape: Assign a section shape to use.

     

    Note

    New Cross I Section and Combined T-Section were incorporated.

     

    ConcreteData: Enter the outer dimensions of the RC section of a steel-encased concrete section.

     

    Steel Data: Enter the steel section data.

     

    User: Enter the main dimensions of a standardized section shape.

     

    H, B1, ...: Refer to the dimension information diagram in the dialog box.

     

    DB: Select a section from the DB of the standard sections for a country.

     

    AISC2K(US): American Institute of Steel Construction, 2000 US Unit : lb, in

     

    AISC2K(SI): American Institute of Steel Construction, 2000 SI Unit : kN, m, mm

     

    AISC: American Institute of Steel Construction

     

    CISC02(US): Canadian Institute of Steel Construction (US Unit : lb, in)

     

    CISC02(SI): Canadian Institute of Steel Construction (SI Unit : kN, m, mm)

     

    BS(S): British Standard

     

    Note

    BS indicates BS4-1 revised prior to 1993.

     

    BS4 - 93: British Standard / BS 4-1 : 1993

     

    DIN(S): Deutches Institut fur Normung e.v

     

    JIS2K : Japanese Industrial Standards 2000

     

    JIS: Japanese Industrial Standards

     

    KS: Korean Industrial Standards

     

    GB-YB: Guojia Biao Zhun-Yejin Bu Biao Zhun

     

    Pacific(SI): Bentley Pacific Standards (SI Unit : kN, m, mm)

     

    IS84: Indian Standards

     

    CNS91: Taiwan Standards

     

    Steel Name: Enter directly a DB section name or select a desired DB from the Section list. When the section name is directly entered, it must correspond to the format of the DB section names.

     

    Ex) AISC: W36x280, BS: UB 406x178x54, DIN: HD400x288, JIS, KS: H 400x200x8/13

     

    Material: Enter material properties for steel and concrete constituting steel RC composite sections.

     

    Click to select the material properties for steel and concrete stored in the DB for a country. The following items are automatically entered:

     

    Es/Ec: Modulus of Elasticity Ratio of steel relative to concrete

     

    Ds/Dc: Specific Weight (Density) Ratio of steel relative to concrete

     

    Ps: Poisson's Ratio for steel

     

    Pc: Poisson's Ratio for concrete

     

    Combined Ratio of Conv.:  Stiffness Reduction Factor of concrete [Default = 1.0]

     

    Note
    When RC is converted into steel for calculating the SRC section stiffness, Conv. Stiffness Factor is applied to reduce the stiffness of RC.

     

    Replace: Assign Steel to be the reference when calculating stiffness of a composite section

     

    Note
    MIDAS/Civil converts RC into equivalent steel for SRC section stiffness calculation.

 

Section - Combined dialog box

 

  •  [Combined tab]

    In this dialog box, enter the section properties for a combined section made up by two standard section types.

     

    User: Enter the main dimensions of standardized section shapes.

     

    DB: Select the sections from the DB of the standard sections for a country.

     

    AISC2K(US): American Institute of Steel Construction, 2000 US Unit : lb, in

     

    AISC2K(SI): American Institute of Steel Construction, 2000 SI Unit : kN, m, mm

     

    AISC: American Institute of Steel Construction

     

    CISC02(US): Canadian Institute of Steel Construction (US Unit : lb, in)

     

    CISC02(SI): Canadian Institute of Steel Construction (SI Unit : kN, m, mm)

     

    BS(S): British Standard

     

    Note

    BS indicates BS4-1 revised prior to 1993.

     

    BS4 - 93: British Standard / BS 4-1 : 1993

     

    DIN(S): Deutches Institut fur Normung e.v

     

    JIS2K : Japanese Industrial Standards 2000

     

    JIS: Japanese Industrial Standards

     

    KS: Korean Industrial Standards

     

    GB-YB: Guojia Biao Zhun-Yejin Bu Biao Zhun

     

    Pacific(SI): Bentley Pacific Standards (SI Unit : kN, m, mm)

     

    IS84: Indian Standards

     

    CNS91: Taiwan Standards

     

    Data 1, Data 2: Enter the section data for individual components constituting the combined section.

     

    Sect. Name: Enter directly a DB section name or select a desired DB from the Section list. When the section name is directly entered, it must correspond to the format of the DB section names.

     

    Ex) AISC: W36x280, BS: UB 406x178x54, DIN: HD400x288, JIS, KS: H 400x200x8/13

     

    H, B, ...: Refer to the diagram denoting section dimensions in the dialog box.

     

    Revision of Gen 2010

     

    Note Applicable composite section DB for design

     

    1. Design code : KSSC-ASD03, AISC-ASD89, TWN-ASD90

    2. Section DB : H-T Combined Shape, 2T(Web Opened H), H-Shape with 2T or Web

 

 

 

Section - Tapered dialog box

 

  • [Tapered tab]

    In this dialog box, enter the section properties for both ends of a line element to define a non-uniform section (Non-prismatic Section/ Tapered Section) of identical shape.(Refer to Note)

     

    Section Shape List: Applicable tapered section shapes are shown below.  For PSC, Composite Type or General Section of Value type, pre-defined sections can be brought in from the Section DB.

     

    DB/User: All sections except for the R-Octagon section

     

    Value: All sections except for the R-Octagon section

     

     

    PSC: All PSC Type sections

     

     

    Composite: Typical 4 composite sections (Steel-Box, Steel-I, PSC-I & PSC-T)

     

     

    Value: Assign value when the user directly enters the section stiffness data.

     

    Enter the section dimensions for section-i and j separately and click . Then, the user may modify the auto-calculated stiffness data or directly enter the stiffness data without entering the section dimensions.

     

    User: Enter the main dimensions of standardized section shapes.

     

    DB: Select the sections from the DB of the standard sections for a country.

     

    AISC2K(US): American Institute of Steel Construction, 2000 US Unit : lb, in

     

    AISC2K(SI): American Institute of Steel Construction, 2000 SI Unit : kN, m, mm

     

    AISC: American Institute of Steel Construction

     

    CISC02(US): Canadian Institute of Steel Construction (US Unit : lb, in)

     

    CISC02(SI): Canadian Institute of Steel Construction (SI Unit : kN, m, mm)

     

    BS(S): British Standard

     

    DIN(S): Deutches Institut fur Normung e.v

     

    JIS2K : Japanese Industrial Standards 2000

     

    JIS: Japanese Industrial Standards

     

    KS: Korean Industrial Standards

     

    GB-YB: Guojia Biao Zhun-Yejin Bu Biao Zhun

     

    Pacific(SI): Bentley Pacific Standards (SI Unit : kN, m, mm)

     

    IS84: Indian Standards

     

    CNS91: Taiwan Standards

     

    Section-i, Section-j: Enter directly each section name corresponding to the starting section-i and the ending section-j or select the desired DB from the section list to describe the tapered section. When the section names are directly entered, they must correspond to the DB section name format.

     

    Ex) AISC: W36x280, BS: UB 406x178x54, DIN: HD400x288, JIS, KS: H 400x200x8/13

     

    y Axis Variation: Dimensional variation affects the moment of inertia about the element local y-axis along the length.

     

    z Axis Variation: Dimensional variation affects the moment of inertia about the element local z-axis along the length.

     

    Linear: linear variation along the element local x-direction

     

    Parabolic: parabolic variation along the element local x-direction

     

    Cubic: cubic variation along the element local x-direction

     

    Note 1

    Calculation of section properties as per Dimensional Variation[Details]

    Once the main section dimensions of both ends of a tapered section member are entered, the section properties are considered to vary from the i end (element connection node N1) to the j end (element connection node N2) along the member length. The cross sectional areas, effective shear areas and torsional resistances are assumed to vary linearly from i to j along the element local x-axis. The moments of inertia are assumed to vary linearly, parabolically or cubically depending on the directions of section changes.

     

    For instance, in the figures below, the variations of Iyy and Izzcan be expressed as follows:

    Moments of Inertia about strong and weak axes for a rectangular section <See figure below>

     

    When the width (B) is constant and the height (H) varies, the moments of inertia show a cubic variation about the strong axis and a linear variation about the weak axis. Namely, Iyy Variation = 'Cubic', IzzVariation = 'Linear'.

    Moments of Inertia about strong and weak axes for an I-section <See figure below>

     

     

    When the width (B) is constant and the height (H) varies, the moment of inertia about the strong axis shows a nearly parabolic variation if the 1st and 2nd terms are neglected in the above equation. The moment of inertia about the weak axis varies almost linearly. Hence, it is feasible to use Iyy Variation = 'Parabolic', IzzVariation = 'Linear'. On the other hand, when the height (H) is constant and the width (B) varies, the moment of inertia about the strong axis varies almost linearly and the moment of inertia about the weak axis shows a nearly cubic variation. Hence, it is feasible to use Iyy Variation = 'Linear', Izz Variation = 'Cubic'.

     

     

    Entry of section data for a tapered section member

     

    Note 2

    In the results produced in contours, diagrams and tables, dimensional variation in the axial direction affects the moment of inertia only. In Beam Detail Analysis, section properties are directly calculated at 1/4, 1/2 and 3/4 points using the shape information. As such, dimensional variation affects all the section properties (A, Asy, Asz, Ixx, Iyy & Izz). 

     

 

 

Section - Composite dialog box

 

  • [Composite tab]

    In this dialog box, the sectional data pertaining to the "Analysis considering the section variation before and after composite actions in Composite Bridges" are specified.

     

    Section Type: Assign a section type

     

     

     

    Steel-Box: Structural steel Box Girder

     

    Steel -I: Structural Steel I Shape Girder

     

    User: Section properties defined as General Section in the Value Tab

     

     

     Slab Width / Girder Num. & CTC

     

    Slab Width: Total width of slab (used for calculating lateral flexure stiffness after becoming composite)

     

    Girder

     

    Num.: Number of girders within the total slab

     

    CTC: Center to center spacing between girders

     

    Note 1

    In case when the number of girders is 1 in a structure, enter 1 for Number of girders (Num) and enter 0 for center to center spacing (CTC).

     

    Note 2 When a number of girders exist

    If a slab width and girder data are entered where a number of  girders exist, the program assumes that the slab acts as a rigid body and increases the moment of Inertia about the vertical direction (Izz).  This concept is shown in Case I and Case II below.

     

     

    In case of a separate section as in Case I and in case of a rigid body section as in Case II, Izz is calculated as below.

     

     

    Slab

     

    Bc: Effective slab width for one girder

     

    tc: Thickness of slab

     

    Hh: Distance from the top of girder to the underside of slab

     

     

    Girder

     

    Steel-Box

    Hw: Height of web excluding flanges

    tw: Thickness of web

    B1: Width of top flange (distance between web centers in Box type)

    B2: Width of bottom flange (distance between web centers in Box type)

    Bf1: Top flange overhang from the center of web in Box type

    Bf2: Bottom flange overhang from the center of web in Box type

    tf1: Thickness of top flange

    tf2: Thickness of bottom flange

    N1: Number of stiffeners on top flange

    Hr1: Height of top flange stiffeners

    tr1: Thickness of top flange stiffeners

    N2: Number of stiffeners on bottom flange

    Hr2: Height of bottom flange stiffeners

    tr2: Thickness of bottom flange stiffeners

     

    Steel-I

    Hw: Height of web excluding flanges

    tw: Thickness of web

    B1: Width of top flange (distance between web centers in Box type)

    B2: Width of bottom flange (distance between web centers in Box type)

    Bf1: Top flange overhang from the center of web in Box type

    Bf2: Bottom flange overhang from the center of web in Box type

    tf1: Thickness of top flange

    tf2: Thickness of bottom flange

     

    User

    Before(After) Composite

    If "User" is selected in Section Type, select Before & After Composite sections.

     

    Section

    Select the section data to be applied s Before/After Composite sections from the section data already defined under other tabs such as DB/User, Value, ect.

     

    Material

     

    Click [Select Material from DB...] button to select the material properties for steel and concrete stored in the DB for a country. The following items are automatically entered.

    Es/Ec: ModulusRatio, steel to concrete

    Ds/Dc: Density ratio, steel to concrete

    Note

    For the calculation of section properties of Composite Section, concrete is converted into steel. The self-weight is computed as follows:

    The Weight of Composite Section =  Steel Weight + Concrete Weight

    If Ds/Dc = 0, concrete weight is ignored and only steel weight is considered.

     

    Ps: Poisso's ratio of steel

    Pc: Poisson's ratio of concrete

    Multiple Modulus of Elasticity

    Recalculate the modulus of elasticity of slab concrete to calculate the stresses due to creep and shrinkage. Multiple elastic modulus ratios need to be inputted into an identical section for different load cases. Application of this to analyses and stress checks is specified in EN1994-2 (Eurocode4: Design of composite steel and concrete structures, Part 2) 5.4.2.2.

    By checking on this option and entering Es/Ec(Long Term) and Es/Ec(shrinkage), the section properties for post-composite section with those modulus ratios taken into account are calculated.

    The value Ixx of the post-composite section is calculated based on the shear modulus ratio (Gs/Gc), not the elastic modulus ratio (Es/Ec). When Es/Ec is entered from DB, Poisson's Ratios from DB are used for the calculation of Gs and Gc. When Es/Ec is inputted by the user, Poisson's Ratio is set to 0.