A Static Analysis Setting (SA) specifies the rules according to which load cases and load combinations are calculated. Three standard analysis types are preset.
Basis
The Basis tab manages the settings for static analysis and elementary calculation parameters.
Analysis type
This section controls the calculation theory used to analyze load cases and load combinations. Three approaches are available for selection in the 'Analysis type' list.
Linear static analysis
When calculating according to the linear static analysis, the equilibrium is examined on the undeformed system. A linear consideration is performed because the deformations of the components are not included in the calculation.
Load cases are calculated linearly according to the linear static analysis by default.
Second-order analysis (P-Δ)
In the "structural" second-order analysis, the equilibrium is determined on the deformed system. The deformations are assumed to be small. Axial forces in the system affect an increase in bending moments. The second-order analysis is therefore used when the axial forces are significantly greater than the shear forces.
Load combinations are calculated nonlinearly according to the second-order analysis by default.
Large deformation analysis
The large deformation analysis ("theory of large deformations") considers longitudinal and transverse forces in the calculation. After each iteration step, the stiffness matrix of the deformed system is created. Loads are treated differently: A load defined in a global direction retains its direction when the finite elements rotate. If the load acts in the direction of a local member or surface axis, it changes its direction according to the rotation of the element.
If the model contains cable members or membrane surfaces, the calculation according to the large deformation analysis is preset.
Iterative method for nonlinear analysis
Depending on the analysis type, various methods are available for solving the nonlinear algebraic equation system.
Newton-Raphson
For the large deformation analysis, the Newton-Raphson method is preset. The nonlinear equation system is solved numerically using iterative approximations with tangents. The tangential stiffness matrix is determined as a function of the current deformation state; it is inverted in each iteration cycle. In most cases, this method achieves rapid (quadratic) convergence.
Newton-Raphson combined with Picard
With this method, the Picard method is used first. After a few iterations, a switch is made to the Newton-Raphson method. The basic idea of this approach is to use the relatively "insensitive" Picard method for the first iteration steps in order to avoid instability messages. With the initial approximation, the fast Newton-Raphson method is then used to find the final equilibrium state.
Picard
The Picard method – also called the secant method – can be understood as a finite difference approximation of the Newton-Raphson method. The difference between the current and the original iteration run in the current load step is considered. This method usually converges more slowly than the Newton-Raphson calculation method. However, it also proves to be less sensitive to nonlinear problems, which makes the calculation more stable.
Newton-Raphson with snap-through problem
This method is suitable for solving snap-through problems where a range with instability must be overcome. If instability exists and the stiffness matrix cannot be inverted, the stiffness matrix of the last stable iteration step is used. Calculations continue with this matrix until the stability range is reached again.
Dynamic relaxation
The last method is suitable for calculations according to the large deformation analysis and for solving snap-through problems. In this approach, an artificial time parameter is introduced. Considering inertia and damping, the problem can then be treated as a dynamic problem. This approach uses the explicit time integration method; the stiffness matrix is not inverted. For a calculation with dynamic relaxation, no part of the model may have a specific weight of zero.
This method also includes Rayleigh damping, which can be defined via the constants α and β according to the following equation with the derivatives with respect to time:
|
M |
Concentrated (diagonal) mass matrix |
|
C |
Diagonal damping matrix C = αM + βdiag[K11(u),K22(u),...,Knn(u)] |
|
K |
Stiffness matrix |
|
f |
Vector of external forces |
|
u |
Discretized displacement vector |
Control elements for nonlinear analysis
The 'Maximum number of iterations' specifies how many calculation runs may occur at most in an analysis according to the second-order or large deformation analysis as well as for nonlinearly acting objects. If the calculation reaches this limit without an equilibrium being established, a corresponding message appears. You can then decide whether the results should be displayed.
The 'Number of load steps' is relevant for analyses according to the second-order or large deformation analysis. When considering large deformations, it is often difficult to find an equilibrium. Instabilities can be avoided by applying the loading in several steps. If you specify two load steps, for example, half of the load is applied in the first step. Iterations are performed until the equilibrium is found. In the second step, the full loading is then applied to the already deformed system and iterations are performed again until equilibrium is reached.
Options I
In this section, you can activate various 'special settings' to influence the calculation according to the second-order or large deformation analysis.
Modify standard precision and tolerance settings
If you check the 'Modify standard precision and tolerance settings' check box, the Precision and Tolerance tab is added to the dialog. There you can adjust the convergence criteria.
Ignore all nonlinearities
With the 'Ignore all nonlinearities' check box, you can deactivate the nonlinear properties of elements for the calculation. Tension members, for example, then remain in the model as soon as compressive forces occur. However, you should only suppress the nonlinear properties for test purposes, for example to find the cause of an instability. Sometimes incorrectly defined failure criteria are responsible for the termination of the calculation.
Options II
Modify loading by multiplication factor
After checking the check box, you can specify a factor k by which all loads are to be multiplied. In older standards, there is a requirement to multiply loads globally by a factor in order to increase the effects according to the second-order analysis for stability analyses. The design, in turn, must be performed with the service loads. Both requirements can be met by entering a factor greater than 1 and activating the 'Divide results by load factor' check box.
For investigations according to current standards, the loading should not be modified by factors. Instead, the partial safety factors and combination coefficients must be considered in the superposition in the design situations.
Consider relieving effect from tension forces in members
Tension forces have a relieving effect on a pre-deformed system. This reduces the deformation and stabilizes the system. This effect is usually utilized in the calculation according to the second-order and large deformation analysis, for example in halls with bracings or generally bending-stressed structures. In the case of underspanned beams, the tension force relief can possibly lead to an undesirable reduction of the deformations and internal forces.
Check stability based on deformation rate
If you check the check box, RFEM checks during the calculation how the deformations develop over the course of the iterations. If the displacements or rotations increase strongly and exceed a program-internal limit, the calculation is terminated with an instability message.
Try to calculate unstable structure
With this check box, an attempt can be made to make an unstable model calculable: RFEM applies small springs in the first calculation step, which stabilize the model for the first iteration. After a stable initial state is reached, these springs are removed again for the following iterations.
Displacements due to member load of the 'Internal pipe pressure' type
The check box is relevant for the member load Internal pipe pressure. The so-called Bourdon effect describes the tendency of a curved pipe to bend straight under the influence of pressure. The circumferential stresses and axial stresses from the internal pressure load lead – considering the material stiffness and transverse strain – to an axial longitudinal strain of the pipe.
A technical article describes in an example how the internal pressure of pipes is calculated.
Save results of all load steps
If the loading is applied incrementally (see section Control elements for nonlinear analysis), you can use the check box to force the output of the intermediate results in order to check the results of the individual load steps.
Unsymmetric direct equation solver
For a nonlinear material model (see chapter Nonlinear material behavior) with unsymmetric properties for tension and compression, an unsymmetric direct equation solver is used. The check box provides the option of using this equation solver for other material models as well, such as for the isotropic nonlinear elastic material model.
Equilibrium for undeformed structure
The check box makes it possible to analyze a structure that does not deform – that is, a system whose deformations remain zero. This analysis option can be useful if, for example, a system is under stress due to a load case, while the resulting deformations can be considered to have subsided.
An application area for calculating the equilibrium for the undeformed structure is the primary stress state of geotechnical analysis. In this case, the stresses acting from the preloading of the soil are to be determined within the scope of a load case or a load combination. However, the deformations of this load case or this combination are not of interest and therefore not subject to further use.
Basic settings
The Basic settings tab manages fundamental specifications for the calculation.
Permanent load ratio
The 'Determine for load combinations' check box provides the option of determining the proportion of a permanent load in a load combination. Select the load combination in the list or create a new load combination with the button
. In the 'Compare result value' list, you can then specify which proportions act statically or variably.
The proportion of the permanent load can be considered according to the standard in the design.
Method for equation system
The selection fields control which method is used to solve the equation system. To avoid misunderstandings: Even with the direct solution of the equation system, an iterative calculation is performed if nonlinearities exist or if the calculation is performed according to the second-order or large deformation analysis. 'Direct' and 'Iterative' refer to the data management during the calculation.
Which equation solver method leads to results faster depends on the complexity of the model as well as on the size of the available main memory (RAM). For small and medium-sized systems, the direct method is more effective. For very large systems, the iterative method leads to results faster.
Plate bending theory
Surfaces can be calculated according to the bending theories of 'Mindlin' or 'Kirchhoff'. When calculating according to Mindlin, shear deformations are included; according to Kirchhoff, these are not considered. The Mindlin calculation option is therefore suitable for the relatively thick plates and shells of solid construction; the Kirchhoff option is recommended for relatively thin surfaces such as steel sheets.
Settings for iterative method
The check boxes of this section are important for the analysis type 'Second-order analysis (P-Δ)'.
Refer internal forces to deformed structure
The internal forces of members are generally output referring to the changed position of the member coordinate systems that exist in the deformed system. If the output is to refer to the undeformed initial system, you can specify the relevant member internal forces by deactivating the corresponding check boxes.
Percentage of iterations according to Newton-Raphson combined with Picard
The Picard solution method is based on secant stiffnesses, the Newton-Raphson method on tangent stiffnesses. For the calculation option Newton-Raphson combined with Picard, secant stiffnesses are used in the first iterations before tangent stiffnesses are applied for the remaining iterations. The proportion of the first iterations with secant stiffnesses is related to the total number of iterations.
Mass conversion into load
Loads can be defined not only as forces and moments, but also in the form of masses. In the static calculation, however, masses have no effect. If they are to be considered, activate the 'Active mass' check box. Then specify the 'Factor in direction' to describe the effect of the mass. The masses are thus converted into forces before the calculation and are included in the determination of the internal forces.
With the button
you can switch between entering the mass factor and the direct specification of the acceleration. The labeling of the input fields is adjusted accordingly.
Reactivation
The Reactivation tab is available as soon as a member with nonlinear properties exists in the model. Here you can control how failing members are treated during the calculation.
Failing members are often the cause of instability problems, for example when a member model is stiffened by tension members. Due to the column shortenings as a result of the vertical load, the tension members receive small compressive forces in the first calculation run. They are removed from the system. In the second run, the model becomes unstable without these tension members. With the options in the 'Reactivation of failing members' section, you can try to achieve a calculation without an error message.
Check deformation of failing members and reactivate them if necessary
RFEM examines the node displacements in each iteration. If, for example, the member ends of a failed tension member move away from each other, the member is used again in the stiffness matrix.
In some cases, reactivating members can be problematic: A member is removed after the first iteration, reinserted after the second iteration, removed again after the third, etc. The calculation would run through this loop until the maximum possible iterations are reached without converging. The 'Maximum number of reactivations' prevents this effect. Here you can specify how often a member element may be reinserted before it is finally removed from the stiffness matrix.
Special treatment
If you check the 'Special treatment' check box, two methods for dealing with failing members are available for selection. They can be combined with the reactivation described above.
- Remove failing members individually one after another in the iterations
After the first iteration, for example, not all tension members with a compressive force are removed at once, but only the tension member with the greatest compressive force. In the second iteration, only one member is then missing in the stiffness matrix. Subsequently, the tension member with the greatest compressive force is removed again. In this way, the system often shows better convergence behavior due to the redistribution effects.
This calculation variant requires more time because a larger number of iterations must be performed. In addition, it must be ensured that a sufficient Maximum number of iterations is provided in the 'Basis' tab.
- Assign very small stiffness to failing members
The failed members are not removed from the stiffness matrix, but a very small stiffness is assigned to them. You can specify this in the 'Reduction factor of stiffness' input field: The factor 1000 means that the member stiffness is reduced to 1/1000.
Precision and Tolerance
The Precision and Tolerance tab provides the option of influencing the convergence and tolerance parameters of the calculation. However, you should only change the default settings in exceptional cases.
Precision of convergence bound for nonlinear calculation
If nonlinear effects are active or the analysis is performed according to the second-order or large deformation analysis, the calculation can be influenced via the convergence bound.
The axial force change of the last two iterations is compared member by member. As soon as this change has reached a certain fraction of the maximum axial force, the calculation ends. During the iterations, however, the case may occur that the axial forces oscillate between two values. You can prevent this pendulum effect by adjusting the "sensitivity".
The precision also affects the convergence criterion for deformation changes in the calculation according to the large deformation analysis, in which geometric nonlinearities are considered. The factor 1.00 is preset. The minimum factor is 0.01, the maximum value is 100.00. The smaller the value, the closer the convergence term must be to the comparison term. The accuracy of the results is increased accordingly.
Tolerance for determination of instability
There are various approaches to investigate the stability behavior of a model. However, none can detect singular stiffness matrices with absolute reliability.
RFEM uses two procedures to determine the instability: On the one hand, the elements on the main diagonal of the stiffness matrix are always compared absolutely with the same number in the iterations. On the other hand, each element of the main diagonal is examined relative to the adjacent number. The tolerance can be adjusted in the input field. The smaller the tolerance value, the closer the instability bound of a model is shifted to the exact instability point. The accuracy of the results is increased accordingly.
Relative setting of time step for dynamic relaxation
The time parameter controls the calculation according to the dynamic relaxation method. The smaller the value, the smaller the time step with which all response fluctuations are recorded. The accuracy of the results is increased accordingly.
Robustness of iterative calculation
In case of convergence problems with the Newton-Raphson method, the robustness can be strengthened to prevent "skipping" the solution. By reducing the value, the number of possible solutions in the presence of a non-converging horizontal solution branch and thus the possibility of a valid result within the specified iterations is reduced. It may be necessary to increase the maximum number of iterations.