Enter section properties for line elements (Truss, Tension-only, Compression-only, 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]
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]
Change element's material number
Section number (Auto-set to the last section number +1)
Up to 999999 Section ID's can be assigned.
Section name (Sect. Name by default if not specified)
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 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.
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 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.
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:
User Offset Reference: Extreme Fiber(s)
Vertical Offset: User, Offset Distance (i & j) = Pier Table section height-Centroid 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 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.
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 , Buckling, Response Spectrum, Construction Stage, Moving Load
Related post-processing: Reactions, Displacements, Beam Forces/Moments, Beam Stresses
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 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
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
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.
Note 4 Element Stiffness data
Sections can be defined by the stiffness data entries even though the section dimensions (H, B1, ... , etc.) are not entered.
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.
Area = +dA = A1 + A2 + A3
= (300 x 15) + (573 x 10) + (320 x 12)
<Figure 1> Example of cross-sectional area calculation
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/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 y-axis direction
Asz: Effective shear area in the ECS z-axis direction
<Figure 2> Effective Shear Area calculations
Torsional resistance refers to the stiffness resisting torsional moments. It is expressed as
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 sub-sections and then their resistances are summed into a total resistance, Ixx, calculated by the equation below.
for a e b
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.
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.
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.
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.
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
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 z-axis
: 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
The area product moment of inertia is used to compute stresses for non-symmetrical sections, which is defined as follows:
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
The following represents a general equation applied to calculate the bending stress of a section:
In the case of an I shaped section, Iyz=0, hence the equation can be simplified as:
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:
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
The first moment of area is used to compute the shear stress at a particular point on a section. It is defined as follows:
When a section is symmetrical about at least one of the y and z-axis, the shear stresses at a particular point are:
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
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.
<Figure 12> Example of calculating a shear factor
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
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.
Let me first discuss the results for the section generated using the Composite Steel-I 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.
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:
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 I-beams have generally poor torsional performance, we can simply use the Composite Steel-I 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.
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:
Q3. When I try to generate a tapered section between two pre-defined sections (both imported from Section Property Calculator), software gives an error message and fails to generate the tapered section. Why?
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 non-zero value for the same section property. To define the tapered section successfully, either the section property should be zero for both the sections or non-zero.
Q4. The principal one is the calculation of the torsional properties. When we use it we calculate them and we modify the values.
For the calculation of torsional constant of Composite Section, Hambly method is used as it is mentioned in the Q1. However, there are slight differences for the calculation of torsional constant of girder section for Composite-PSC section and Composite-Steel sections.
Steel-Box : Ixx = Ixx_girder (Bredt Formula)+ Ixx_slab
Steel-Tub : Ixx = Ixx_girder (Bredt Formula)+ Ixx_slab
Steel-I : Ixx = Ixx_girder (General Formula)+ Ixx_slab
Composite-I, T, PSC, General : Ixx = Ixx_girder(Finite Element Method) + Ixx_slab
Bredt formula represents torsional constant calculation method for thin wall closed section. General Formula represents torsional constant calculation method by breaking up into thin rectangles as described in Q1. FEM is the same method which is used for the calculation of torsional constant of SPC section.
These can cause inevitable differences in terms of torsional constant value in certain cases such as Tub section for the Composite-Steel and Composite-PSC.
For the calculation of torsional constant before composite action, the program assumes that tub section is closed before slab concrete is hardened. During erection in practice, lateral bracings are attached to top flanges in tub girder as shown below.
Top flange lateral bracing creates a quasi-closed section, which increases the torsional stiffness of tub girder sections during erection, handling, and deck casting. The top flange lateral bracing forms a quasi-closed section resisting shear flow from the non composite loading. This reflects the practice in the US. If you need to apply any different values of torsional constant, you need to use Section Stiffness Scale Factor. Figure below shows the one of the example comparing tub section Ixx and SPC calculation by modeling it as closed box. When we consider it as closed box, torsional stiffness is almost same.
After composite action, the value Ixx is calculated based on the shear modulus ratio (Gs/Gc). 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.
In this case, Ixx_girder is calculated by assuming it as closed section. The torsional constant for closed section used in midas Civil can be found in the following online help.
In case of Composite-PSC, this can be problematic if the girder section is tub section. Current method of calculation of Ixx of composite section in Civil cannot recognize whether the section is closed or not. Therefore there can be discrepancy when the girder is tub section which makes the whole section as closed section after the composite action. This limitation can be solved by modifying Stiffness Scale Factor of torsional constant manually by the user. This method is also described in Q1, please refer to the Q1 for the details.