## Function

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

## Call

From the main menu, select **[Properties] tab > [Section Properties] group > [Section Properties]**

## Input

Properties(Section) dialog box

### To enter new or additional section properties

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

The section number can be entered up to a maximum of six digits. [999999]

### Modification of previously entered section data

Select the section to be modified from the list in the Section dialog box and click **Modify...** 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 **Delete**.

### To copy previously entered section data

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

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

Click **Import** and select the MCB file containing the section data or specify a file name then click .

**Section List**

The section data inputted in the existing fn.MCB file is displayed.

**Selected List**

Select the section data you want to import and register it in the list.

When selecting fn.MCB, all the existing section data inputted in fn.MCB is registered in the Selected List.

**Numbering Type**

Specify the import method for the section number.

**Keep ID**

Import the section numbers from the existing fn.MCB file using the same numbering scheme.

**New ID**

Assign new numbers to the section data being imported.

### 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 **Renumber**.

**Start number**

Enter the starting number for the section numbers to be changed.

**Increment number**

Enter the increment value for the section property data numbers.

**Change element's material number**

Change the section numbers of the elements. By using this function, the defined section numbers will be modified. If this function is not used, the selected existing section numbers will be converted to an "Undefined" state without a section name defined, and additionally, a user-specified material number will be created for the elements without any section assignment.

Section data definition dialog box

### Section ID

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

Up to 999999 Section ID's can be assigned.

### Name

The section name will be automatically assigned as "Sect. Name" if no input content is provided.

### Consider Shear Deformation

Select whether to consider shear deformation. This option is applied during structural analysis and does not affect the effective shear area (Asy, Asz) data that appears when clicking the **Show Calculation Results...** button.

### 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.

Change Offset dialog box

Offset location

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

**Center Loc.** : Choose the position of the center between the centroid and the center of section dimensions.

**Horizontal Offset** : Specify the lateral offset position of the section. If "to Extreme Fiber" is selected, the position specified in "Offset" will be reflected as shown in the illustration above. If you want to specify an arbitrary position as the offset location, select "User" and enter the offset distance. However, if the offset option is set to "Center-Top/Center/Bottom," the lateral offset position will be fixed at the center, and the "User" option cannot be specified. If it is a variable section, the input field for the J-section will be activated.

**Vertical Offset** : Specify the vertical offset position of the section. If "to Extreme Fiber" is selected, the position specified in "Offset" will be reflected as shown in the illustration above. If you want to specify an arbitrary position as the offset location, select "User" and enter the offset distance. However, if the offset option is set to "Left/Center/Right-Center," the vertical offset position will be fixed at the center, and the "User" option cannot be specified. If it is a variable section, the input field for the J-section will be activated.

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

Node-based loads such as Nodal Loads and Specified Displacements are always applied at the nodes. However, element-based loads such as Beam Loads and Temperature Loads are applied on the center line of the element section. Please find the difference in the following example.

**User Offset Reference** : When entering the offset distance for the section as the "User" type, you can specify the reference position that serves as the basis.

**Centroid** : Apply the offset distance entered based on the centroid of the section.

**Extreme Fiber(s)** : Apply the offset distance entered based on the position specified in "Offset" (Left/Right, Top/Bottom).

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"

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

**- 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 Offset Point** : Display the offset position entered in the Change Offset dialog in the illustration of the Section Data dialog.

### 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 **Show Calculateion Results**.

### Consider Warping Effect (7th DOF)

Select whether to consider warping effect. In case of non-uniform torsion which occurs when warping deformation is constrained, torque is resisted by St.Venant torsional shear stress & warping torsion. The effects of warping torsion can be simulated in 1D beam elements for more accurate results in case of the curved member, eccentric loading, and difference in centroid and shear center.

When “Consider Warping Effect(7th DOF)” is considered, warping constant (Iw), warping function (w1, w2, w3, w4), and shear strain due to twisting moment (γxy1, γxy2, γxy3, γxy4, γxz1, γxz2, γxz3, γxz4) can be checked in Section Properties dialog box.

Applicable element types, boundary conditions and analysis type

Applicable element type : General beam/Tapered beam

Applicable boundary condition : Supports, Beam End Release

Applicable analysis type : Linear Static , Eigenvalue , Buckling, Response Spectrum, Construction Stage, Moving Load

Related post-processing : Reactions, Displacements, Beam Forces/Moments, Beam Stresses

**Warping Check**

The locations for the maximum normal stresses and shear stresses due to warping are automatically identified for the PSC section type including tapered PSC section. The locations can be viewed from the Section Manager dialog. Two points for the maximum/minimum normal stresses and four points for the maximum/minimum shear stresses in the xy and xz plane due to warping.

**Auto**

Six critical points are found by the program.

**User**

Six points can be defined by the user for which stresses are computed.

### Section Property

Click **Show Calculation Results...** 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.

**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 constant 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

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

**Zzz** : Plastic Section Modulus about the element 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 1 (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

**Iw** : Warping constant

**w1, w2, w3 and w4** : Warping function at point 1, 2, 3 and 4 respectively

**Cxy1, Cxy2, Cxy3, Cxy4, Cxz1, Cxz2, Cxz3 and Cxz4** : Coefficients to be used to calculate twisting moment and warping moment

**ys-yc** : Distance between centroid and shear center in the local y direction

**zs-zc** : Distance between centroid and shear center in the local z direction

**Ip** : Polar moment of inertia

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

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.

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. In the case of the Ultimate condition, Pc (compressive), Pt (tensile), and M0 (bending strength at P=0, calculated as Fy×Zyy, Fy×Zzz) are used to generate the PM-Curve.

Element Stiffness data

**Area : Cross Sectional Area**

**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 Civil 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.

<Figure 1 > Example of cross-sectional area calculation

**Asy, Asz : Effective Shear Area**

**Asy, Asz : Effective Shear Area**

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 calculating section properties internally or when they are inputted from a database, the corresponding shear stiffness component is automatically considered, and the calculation method is as shown in Figure 2.

**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 in the ECS z-axis direction

**Ixx: Torsional Constant**

**Ixx: Torsional Constant**

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

<Eq. 1>

where, I_{xx} : Torsional Constant

T : Torsional Moment or Torque

G : Shear Modulus of Elasticity

θ : 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.

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.

<Eq. 2>

where, i_{xx} : 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, Am : Area enclosed by the mid-line of the tube

d_{s} : 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.

<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 sections**

<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 closed and open sections

<Figure 8> Torsional resistance of built-up sections

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

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

<Eq.4>

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

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

<Eq.5>

**The total resistance of the built-up section**

**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> Torsional resistance of built-up sections

**Iyy, Izz: Area Moment of Inertia**

**Iyy, Izz: Area Moment of Inertia**

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.

**Moment of inertia about the y-axis in the element coordinate system**

<Eq. 1>

**Moment of inertia about the z-axis in the element coordinate system**

<Eq. 2>

<Figure 9> Example of the calculation for moment of inertia

**Iyz: Area Product Moment of Inertia**

**Iyz: Area Product Moment of Inertia**

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

<Eq. 1>

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:

In the neutral axis, the bending stress due to the bending moment is '0', allowing us to determine the direction of the neutral axis using the following relationship.

<Eq. 2>

The general equation applied to calculate the bending stress in a section due to bending moment is as follows.

<Eq. 3>

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

<Eq. 4>

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

** Izz** : Area moment of inertia about the ECS y-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. 5>

<Eq. 6>

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

**Qy, Qz: First Moment of Area**

**Qy, Qz: First Moment of Area**

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. 1>

<Eq. 2>

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

<Eq. 3>

<Eq. 4>

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

**Qyb, Qzb: Shear Factors of Shear Stress due to Bending**

**Qyb, Qzb: Shear Factors of Shear Stress due to Bending**

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. 1>

<Eq. 2>

<Figure 12> Example of calculating a shear factor

**Stiffness of Composite Sections**

**Stiffness of Composite Sections**

midas Civil 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 structural steel

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**

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

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.