Considering Second-Order Theory in Dynamic Analysis

Technical Article

For the ultimate limit state design, EN 1998‑1 [1], Section 2.2.2 and 4.4.2.2, require the calculation considering the second‑order theory (P‑Δ effect). This effect need not be taken into account only if the interstorey drift sensitivity coefficient θ is less than 0.1.

The coefficient θ is defined as follows:

$$\mathrm\theta\;=\;\frac{\displaystyle{\mathrm P}_\mathrm{tot}\;\cdot\;{\mathrm d}_\mathrm r}{{\mathrm V}_\mathrm{tot}\;\cdot\;\mathrm h}\;\;\;\;\;\;\;\;\;\;\;(1)$$

where

θ  is the interstorey drift sensitivity coefficient
Ptot  is the total gravity load at and above the storey considered in the seismic design situation (see Expression 2)
dr  is the design interstorey drift, evaluated as the difference of the average lateral displacements dS at the top and bottom of the storey under consideration; for this, the displacement is determined by using the linear design response spectrum with q = 1.0
Vtot  is the total seismic storey shear determined by using the linear design response spectrum
is the interstorey height

The second-order effects may approximately be taken into account by a factor equal to 1 / (1 − θ), if 0.1 < θ ≤ 0.2. For θ > 0.2, it is necessary to consider the geometric stiffness matrix when calculating eigenvalues and multi-modal response spectrum analysis.

Geometric Stiffness Matrix

For dynamic analyses, the iterative calculations for the nonlinear determination of second‑order theory are not suitable. The problem can be linearised, and it is sufficient to use the geometric stiffness matrix based on axial loads to consider the second‑order theory. For this, it is assumed that the vertical loads do not change due to horizontal effects and the deformations are small compared to the building dimensions [2]. The loads to be considered should correspond to those for the seismic design situations in accordance with EN 1990, Section 6.4.3.4 [3]:

$${\mathrm E}_\mathrm d=\sum_{\mathrm j\geq1}{\mathrm G}_{\mathrm k,\mathrm j}+\sum{\mathrm\Psi}_{2,\mathrm i}{\mathrm Q}_{\mathrm k,\mathrm i}\;\;\;\;\;\;\;\;\;\;(2)$$

where

Ed  is the design value of the effects
Gk,j  is the characteristic value of a permanent action j
Qk,i  is the characteristic value of a variable action i
Ψ2,i  is the factor for quasi‑permanent values of variable actions i

Axial tensile forces increase the stiffness, for example, in a prestressed cable. Compression forces reduce the stiffness and can lead to a singularity in the stiffness matrix. The geometric stiffness Kg is not dependent on mechanical properties of the structure, but only on the member length L and axial force N.

To illustrate the basic problem, there is a simple example of a cantilever displayed in Figure 01. The single mass points of the cantilever represent the individual storeys of a building. The building is subjected to a dynamic analysis considering the second‑order theory. The axial forces Ni on the individual storeys i = 1...n result from the vertical forces in the seismic design situation (see Expression 2). The storey height is defined by hi.

Figure 01 - Reduction of building on cantilever structure. The individual mass points represent storeys. Displacement due to compression normal forces shown in (a) is converted to (b) overturning moments or lateral loads [2].

The geometric stiffness matrix Kg can be derived from the static equilibrium conditions:

$$\begin{bmatrix}{\mathrm F}_\mathrm i\\{\mathrm F}_{\mathrm i+1}\end{bmatrix}\;=\;\underbrace{\frac{{\mathrm N}_\mathrm i}{{\mathrm h}_\mathrm i}\left[\begin{array}{rc}1.0&\;-1.0\\-1.0&\;1.0\end{array}\right]}_{{\mathbf K}_\mathbf g}\;\begin{bmatrix}{\mathrm u}_\mathrm i\\{\mathrm u}_{\mathrm i+1}\end{bmatrix}\;\;\;\;\;\;\;\;\;\;(3)$$

For the purpose of simplification, only the degrees of freedom of the horizontal displacement are displayed here. The derivation shown is based on the overturning moment approach due to the linear displacement application. This is a simplification for the bending element, and an accurate assumption for the truss element.

More precise determination of the geometric stiffness matrix for bending beams can be obtained by using the cubic displacement approach or the analytical solution of the differential equation of the bending line. More information and derivations are provided by Werkle [4].

The geometric stiffness matrix Kg is added to the system stiffness matrix K, and thus the modified stiffness matrix Kmod is obtained:

$${\mathbf K}_\mathbf{mod}\;=\;\mathbf K\;+\;{\mathbf K}_\mathbf g\;\;\;\;\;\;\;\;\;\;(4)$$

In the case of compression normal forces, this consequently leads to the stiffness reduction.

Example: Natural Frequencies and Multi-Modal Response Spectrum Analysis Considering Second-Order Theory

The following shows how the geometric stiffness matrix can be considered in RFEM and the RF‑DYNAM Pro add‑on modules. As an example, the cantilever shown in Figure 01 is used. The cantilever consists of five concentrated mass points. Here, 4,000 kg act in the global X‑direction in each case.

Figure 02 - Self-weight and imposed loads are summarised as nodal loads and defined in two separate load cases.

The cross‑section is IPE 300 made of the material S 235 with:
${\mathrm l}_\mathrm y\;=\;8.356\;\cdot\;10^{-5}\;\mathrm m^4\;$
$\mathrm E\;=\;2.1\;\cdot\;10^{11}\;\mathrm N/\mathrm m^2$
To be able to consider the geometric stiffness matrix in the dynamic analysis, a load combination is initially defined for the seismic design situation in the main program RFEM (see Equation 2).

Figure 03 - Definition of the load combination for the seismic design situation (Expression 2) and the resulting axial forces. These axial forces are used to determine the geometric stiffness matrix.

The RF‑DYNAM Pro - Natural Vibrations add‑on module allows you to determine natural frequencies, mode shapes and effective modal masses of a structure, taking into account various stiffness modifications (see RF‑DYNAM Pro Manual [5], Chapter 2.4.7, and Technical Article [6]). Two natural vibration cases are defined. In NVC2, CO1 is imported in order to consider the geometric stiffness matrix and thus the second‑order theory. For comparison, the NVC1 is defined, which does not include any stiffness modifications.

Figure 04 - Parameters for Eigenvalue Analysis in RF‑DYNAM Pro - Natural Vibrations

The following table includes the determined natural frequencies f [Hz], natural periods T [sec], and the acceleration values Sa [m/s²] based on the response spectrum, with and without the geometric stiffness matrix Kg resulting from the axial forces of CO1.

Figure 05 - Natural Frequencies, Periods and Acceleration Values

The multi-modal response spectrum analysis uses natural frequencies to determine the acceleration values from the defined response spectrum. Based on these acceleration values, the equivalent loads and the response spectrum internal forces are determined. The graphic display of a user‑defined response spectrum is shown in Figure 06, and the acceleration values Sa [m/s²] determined from the response spectrum for each eigenvalue are listed in the table above.

Figure 06 - User-Defined Response Spectrum

In order to ensure the correct allocation of the modified frequencies, the right natural vibration case (NVC) must be assigned to the dynamic load case (DLC).

Figure 07 - Assigning Natural Vibration Case to Dynamic Load Case to Determine Equivalent Loads

In the case of compression axial forces, the consideration of the geometric stiffness matrix leads to the reduction of the natural frequency, and can cause lower acceleration values Sa, such as in our example. Sole modification of the natural frequencies is not enough to consider the second‑order theory. In fact, this may actually lead to smaller results, which can be thus incorrect. It is very important to also use the modified stiffness matrix for the determination of internal forces and deformations.

In RF-DYNAM Pro - Forced Vibrations, the modified stiffness is automatically used to determine the response spectrum results, because the calculation is performed within RF‑DYNAM Pro. InRF‑DYNAM Pro - Equivalent Loads, the equivalent loads are determined and exported as load cases into the main program RFEM. Therefore, the calculation is performed partially in RF‑DYNAM Pro and partially in RFEM.

Theoretical background for the equivalent load calculation is explained in the Manual RF‑DYNAM Pro [5]. The verification example [7] shows the calculation on a specific example. The determined equivalent loads, with and without the geometric stiffness matrix, are displayed in Figure 08.

Figure 08 - Equivalent loads for Mode Shape 1 (a) without stiffness modifications from DLC1 and (b) with geometric stiffness matrix from DLC2

The export of the equivalent loads has many advantages, but the most important is the correct transfer of stiffness modifications in the load cases. The calculation parameters of the exported load cases must be adjusted as shown in Figure 09.

Figure 09 - Calculation parameters of load cases with the exported equivalent loads. Here also, the geometric stiffness matrix must be considered. For this, the axial forces from LC1 are imported.

The individual load cases are superimposed using the SRSS or CQC method. This is automatically set in RF‑DYNAM Pro and exported into result combinations. The results with and without the geometric stiffness matrix are displayed in Figure 10.

Figure 10 - Deformations uX, moment MY, and support reactions PX resulting from the multi-modal response spectrum analysis (a) with no stiffness modifications from DLC1 and (b) with the geometric stiffness matrix from DLC2

The consideration of the geometric stiffness matrix leads to larger deformations and internal forces. However, the equivalent loads and resulting support loads are slightly smaller when considering the geometric stiffness matrix.

Reference

[1]   Eurocode 8: Design of structures for earthquake resistance - Part 1: General rules, seismic actions and rules for buildings; EN 1998‑1:2004 / A1:2013
[2]   Wilson, E. (2002). Three dimensional static and dynamic analysis of structures. Berkeley, Calif.: Computers and Structures Inc.
[3]   Eurocode 0: Basis of structural design; EN 1990:2010‑12
[4]   Werkle, H. (2008). Finite Elemente in der Baustatik: Statik und Dynamik der Stab- und Flächentragwerke (3rd ed.). Wiesbaden: Springer Vieweg.
[5]   Manual RF-DYNAM Pro. (2016). Tiefenbach: Dlubal Software. Download.
[6]   Schubert, G. (2015). Import of Axial Forces, Stiffness Modifications and Extra Options in RF-/DYNAM Pro - Natural Vibrations. Tiefenbach: Dlubal Software.
[7]   Verification Example 105: Equivalent Loads. (2015). Dlubal Software website. Download.

Links

Contact us

Contact to Dlubal

Do you have any questions or need advice?
Contact us or find various suggested solutions and useful tips on our FAQ page.

+49 9673 9203 0

info@dlubal.com

RFEM Main Program
RFEM 5.xx

Main Program

Structural engineering software for finite element analysis (FEA) of planar and spatial structural systems consisting of plates, walls, shells, members (beams), solids and contact elements

RFEM Dynamic Analysis
RF-DYNAM Pro - Natural Vibrations  5.xx

Add-on Module

Dynamic analysis of natural frequencies and mode shapes of member, surface, and solid models

RFEM Dynamic Analysis
RF-DYNAM Pro - Forced Vibrations 5.xx

Add-on Module

Dynamic and seismic analysis including time history analysis and multi-modal response spectrum analysis

RFEM Dynamic Analysis
RF-DYNAM Pro - Equivalent Loads 5.xx

Add-on Module

Seismic and static load analysis using the multi-modal response spectrum analysis