Section



Enter section properties for line elements (Truss, Tensiononly, Compressiononly, Cable, Gap, Hook, Beam Element). 



From the Main Menu select Properties > Section > Section Properties. 


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 Selected List Note Numbering Type Keep ID New ID 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] Start number Increment Change element's material number
Section ID Section number (Autoset 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]
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 outermost 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 "CenterCenter" the Horizontal Offset can be entered as the "User" type. For a tapered (nonprismatic) section, data input for the Jend also becomes activated. Vertical Offset: Specify the Offset in the vertical direction. "to Extreme Fiber" assigns the offset to the outermost point. For a specific location of Offset, select "User" and enter the distance from "Centroid" to the desired Offset location. Unless the Offset is "CenterCenter" the Vertical Offset can be entered as the "User" type. For a tapered (nonprismatic) section, data input for the Jend also becomes activated. Note 1 When Offset distance is specified, a positive (+) sign applies to Centertooutward for Centroid reference and Extremetoinward for Extreme Fiber reference.
Note 2 Nodebased loads such as Nodal Loads and Specified Displacements are always applied at the nodes. However, elementbased 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 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 3 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: LeftCenter", "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 "LeftCenter" 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 4 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: CenterTop User Offset Reference: Extreme Fiber(s) Vertical Offset: User, Offset Distance (i & j) = Pier Table section heightCentroid of Pier Table section
: 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 . Consider Warping Effect (7th DOF)Select whether to consider warping effect. In case of nonuniform 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.
Note. 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 , Response Spectrum, Construction Stage Analysis Related postprocessing: Reactions, Displacements, Beam Forces/Moments, Beam Stresses
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 ydirection It becomes inactive when Shear Deformation is not considered. Asz: Effective Shear Area for shear force in the element's local zdirection It becomes inactive when Shear Deformation is not considered. Ixx: Torsional Resistance about the element's local xaxis Iyy: Moment of Inertia about the element's local ydirection Izz: Moment of Inertia about the element's local zdirection Cyp: Distance from the section's neutral axis to the extreme fiber of the element in the local (+)ydirection Cym: Distance from the section's neutral axis to the extreme fiber of the element in the local ()ydirection Czp: Distance from the section's neutral axis to the extreme fiber of the element in the local (+)zdirection Czm: Distance from the section's neutral axis to the extreme fiber of the element in the local ()zdirection Qyb: Shear Coefficient for the shear force applied in the element's local zdirection Qzb: Shear Coefficient for the shear force applied in the element's local ydirection 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 ydirection Zzz: Plastic Section Modulus about the element local zdirection 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. The crosssectional 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. Crosssectional 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. Area = +dA = A1 + A2 + A3 = (300 x 15) + (573 x 10) + (320 x 12) = 14070 <Figure 1> Example of crosssectional 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 zaxis directions of the crosssection. If the effective shear areas are omitted, the shear deformations in the corresponding directions are neglected. When MIDAS/Civil 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 yaxis direction Asz: Effective shear area in the ECS zaxis direction <Figure 2> Effective Shear Area calculations 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 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. For calculating the torsional resistance of an open section, an approximate method is used; the section is divided into several rectangular subsections 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) subsection 2a: Length of the longer side of a subsection 2b: Length of the shorter side of a subsection Figure 3 illustrates the equation for calculating the torsional resistance of a thin walled, tubeshaped, closed section. <Eq. 3>
where, A: Area enclosed by the midline 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, tubeshaped, 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 builtup 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 builtup section. For example, a double Isection 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 builtup section <Eq. 6>
Figure 8(b) shows a builtup section made up of an Ishaped 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 builtup 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 yaxis <Eq. 8>
Area moment of inertia about the ECS zaxis <Eq. 9>
: area : distance from the reference point to the centroid of the section element in the zaxis direction : distance from the reference point to the centroid of the section element in the yaxis direction : first moment of area relative to the reference point in the yaxis direction : first moment of area relative to the reference point in the zaxis 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 nonsymmetrical 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 nonsymmetrical 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 nonsymmetrical section
The neutral axis represents an axis along which bending stress is 0 (zero). As illustrated in the righthand side of Figure 11, the naxis represents the neutral axis, to which the maxis 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 yaxis Izz: Area moment of inertia about the ECS zaxis Iyz: Area product moment of inertia y: Distance from the neutral axis to the location of bending stress calculation in the ECS yaxis direction z: Distance from the neutral axis to the location of bending stress calculation in the ECS zaxis direction My: Bending moment about the ECS yaxis Mz: Bending moment about the ECS zaxis The general expressions for calculating shear stresses in the ECS y and zaxes are: <Eq. 14>
<Eq. 15>
where, Vy: Shear force in the ECS yaxis direction Vz: Shear force in the ECS zaxis direction Qy: First moment of area about the ECS yaxis Qz: First moment of area about the ECS zaxis by: Thickness of the section at which a shear stress is calculated, in the direction normal to the ECS zaxis bz: Thickness of the section at which a shear stress is calculated, in the direction normal to the ECS yaxis 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 zaxis, the shear stresses at a particular point are: <Eq. 18>
<Eq. 19>
where, Vy: Shear force acting in the ECS yaxis direction Vz: Shear force acting in the ECS zaxis direction Iyy: Area moment of inertia about the ECS yaxis Izz: Area moment of inertia about the ECS zaxis by: Thickness of the section at the point of shear stress calculation in the ECS yaxis direction bz: Thickness of the section at the point of shear stress calculation in the ECS zaxis 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/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 crosssectional 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) Revision of Ver.7.4.0  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


Answer: Let me first discuss the results for the section generated using the Composite SteelI option in Civil. The torsion of such sections is calculated using a method where the section is broken down into rectangles, the torsional constant of each of them is calculated and then the torsion of the combined section is a sum of all the parts. In ‘Bridge Deck Behavior’ by E.C. Hambly we can find detailed information on this approach and how to calculate the torsional constant for a single rectangle: And
complex sections can be divided in the following manner to
be calculated as rectangles: Using this approach we can break your section into 4 parts – bottom flange, web, top flange and slab. Each of those is a thin rectangle and we can apply (2.18) to obtain the torsional constants and then combine them to get the resistance of the composite section (using a modular ratio to convert the contribution of the concrete). In case of composite girders where the slab is continuous and only part of it is effective for the composite action with the steel girder, one more consideration has to be taken into account. The normal distribution of torsion has the following pattern:
However, for continuous slabs the vertical components at the two ends of the slab are not present for the general case of intermediate girders and the torsional resistance is better approximated by:
Now using (2.18) for the beam parts and (3.15) for the slab we can carry out a manual calculation. Before composite: and after composite: Now if we look at the values provided by the software you will see these match very well.
Now let’s move on to the SPC section. The first thing that needs to be pointed out is that SPC is a tool for calculation of section properties for arbitrary sections, however, as such it has to work for the general case. As I said in my previous email the way SPC calculates section properties is by performing finite element analysis applying unit loads. But when we analyse a composite beam which has a part of a continuous slab acting as flange, the software cannot take into account the reduced torsional resistance of the slab (formula 3.15) as it analyses the beam as a separate unit. So to check the results manually, we have to use (2.18) for the slab as well: Manual calculation after composite: SPC: Again, we observe a good match between the values for Ixx after composite. The only significant discrepancy is between the ‘before composite’ values. The Composite Steel – I section gives 1.00E7, while SPC gives 1.2E7. This difference is purely due to the accuracy of the approach using the formulae. After all, this is an approximate method and some inaccuracy is normal. For example, some torsional resistance is lost depending on the division of the section into rectangles as we lose resistance along the dividing lines. Hambly provides a good illustration of this: You can easily see how splitting the section in this case reduces the value of the resistance obtained. Now that it is clear where the difference in the values is coming from, it is up to engineers to choose what approach they want to use to. As a solution for most accurate calculation I can suggest to use the SPC feature to generate the section with the exact properties and then apply a factor of 0.5 for Ixx for the slab in the Composite Section for Construction Stage definition.
However, as Ibeams have generally poor torsional performance, we can simply use the Composite SteelI section and neglect the inaccuracy of the torsion of the I section as its contribution to the composite properties is negligible (two orders of magnitude lower than the one of the slab). However, if the structure is such that the effects of torsion before composite are important it may be reasonable to go for the more accurate solution with SPC which I suggested above. I hope this clarifies the topic and you will find this information useful. If there is anything else we could help you with, please let us know. Kind regards, MIDAS Support Answer: The difference is coming from the way torsional stiffness is calculated using approximating methods (that is, the equation option). In midas Civil the section properties are calculated using approximating simplified methods, while SPC can run an FEM analysis of the section to obtain the section properties. Before continuing with this question please read the answer to Q1. Now that it is clear how the two methods work, it is easy to see why the equation option provides much lower results. In this case, as SPC does not support curved lines, the circular parts of the section are represented by a number of straight lines. When we calculate the torsional constant using ‘equation’ the software simply applies the formula for each rectangle (line with thickness) and then sums those up. Obviously, this is incorrect as it completely ignores the connectivity of the lines and the global enclosed shape which the section has and the torsional stiffness which we get is very low. For this reason we have provided an extra function to define the correct stress flow path in such enclosed polygons so that the section properties are calculated correctly. This is done using closed loops (Model > Curve > Closed Loop > Register in SPC). Select the lines on the outer perimeter of the steel section and click apply:
Once this is defined, the torsional constant will be correctly calculated using the equation method as well:
Answer: There could be two scenarios: 1)
Section Properties cannot be calculated for the defined tapered
section: If this is the case then there could be two possible
reasons as mentioned below. 2) Section properties can be calculated but section cannot be defined: This could occur when one of the two predefined sections has zero value for some section property and the other section has nonzero value for the same section property. To define the tapered section successfully, either the section property should be zero for both the sections or nonzero. 
