In addition to our technical support (e.g. via chat), you’ll find resources on our website that may help you with your design using Dlubal Software.
Frequently Asked Questions (FAQ)
Search FAQ
Further Information
Customer Support 24/7

Answer
Yes, you can consider the static rest position in a time history analysis. For this you can use the 'Stationary State' function (not available in the linear modal analysis).
With this function, it is possible to read a condition from a load case or a load combination that exists over the entire time history. These include the deformations, the stiffness modifications, and the states of nonlinearities.This function is activated in the RF/DYNAM Pro addon module, in the 'Calculation Parameters' tab of the Dynamic Load Cases.The time history diagram is well suited for results evaluation. In the attached example, load case 1 with the dead load was defined as a stationary state. In the time diagram, it can be seen that the deformations oscillate about the value that is reached by the static rest position. 
Answer
No, this option does not necessarily have to be activated to consider the dead load. If the masses are imported from a load case that already contains the dead load, it is not necessary to activate this option. Otherwise, the dead load of the structure will be doubled. 
Answer
The differences between the two modules are explained in this FAQ.
In the case of the same settings, there should also be the same results calculated in both addon modules. However, this does not apply to the existing nonlinearities. The reason is that there are no nonlinearities considered in the RF‑/DYNAM Pro addon module. If displaying the results in the Forced Vibrations addon module, all nonlinearities are thus ignored. In contrast, the equivalent loads are calculated on a linear structural system, but the exported load cases are then calculated on a real structure in RFEM and RSTAB, that is, with all nonlinearities. This may lead to inconsistent results.
If you deactivate the nonlinearities for the exported load cases, you should obtain the same results.
The way of considering nonlinearities in the response spectrum analysis is described on the basis of tension members in this FAQ.

Answer
There can be many reasons for the small effective modal mass factors. This can often be observed in the case of large structures. In most cases, the reason for this problem is the fact that only local mode shapes occur. The following text describes how you can handle this: You should recognize from the result graphic whether the local mode shapes are really there. If the individual members or surfaces have a very low natural frequency, these occur first.
 In the case of including these local eigenvectors in the calculation anyhow, you should increase the number of mode shapes to be calculated.
 If the local mode shapes occur on surfaces, the masses of the affected surfaces can be neglected. This feature is described in this technical article.
 In the case of the local mode shapes on members, it is recommended to deactivate the FE mesh division on members.
If you have paid attention to all of these notes, the global mode shapes of the structure should only be activated, which also activate a high mass. 
Answer
There are two options available: an automatic time step selection and a manual one. Especially for a structure with nonlinearities, it is always recommended to select the time step manually, because the automatic determination is only carried out on the basis of the defined accelerograms or time diagrams. For this purpose, a time step convergence study should be performed, which compares the calculation time and the accuracy.
The time step to be selected depends on many factors, including the excitation frequency, the frequency and the size of the structure, as well as the degree of nonlinearities. Thus, it is not possible to make a general statement about the size of the time step.
To achieve sufficient accuracy, the governing period T = 1/f should be divided into approximately 20 steps, that is, the time step Δt should be selected as follows:
$\mathrm{Δt}\;<\frac{\mathrm T}{20}\;=\;\frac1{20\mathrm f}\;=\;\frac{\mathrm\pi}{10\mathrm\omega\;}$
For transiently defined suggestions, such as accelerograms or tabulated time diagrams, the shortest time period should be divided into 7 steps:
$\mathrm{Δt}\;=\;\frac{\mathrm{Min}\left\{{\mathrm t}_{\mathrm i+1}\right.\;{\mathrm t}_{\mathrm i}\}\;}7$
Regardless of the calculation, time steps are specified to save the results.

Answer
The RFDYNAM Pro  Nonlinear Time History offers, in addition to the implicit NEWMARK method of mean acceleration, also an explicit method. In the manual of this addon module, it is mentioned that this is a solver which uses the central difference method.
It should be noted that not the "original" version of the central difference method is used here, but a modified form. The modified form is characterized by the fact that it is simply not a central difference when applying the speed difference. The following two equations show the applied speed and acceleration differences.
Speed: (no central difference)${\dot{\mathrm x}}_{\mathrm n+\frac12}=\frac{{\mathrm x}_{\mathrm n+1}{\mathrm x}_\mathrm n}{{\mathrm{Δt}}_{\mathrm n+{\displaystyle\frac12}}}$
Acceleration: (central difference)${\ddot{\mathrm x}}_\mathrm n=\frac{{\dot{\mathrm x}}_{\mathrm n+{\displaystyle\frac12}}{\dot{\mathrm x}}_{\mathrm n\frac12}}{{\mathrm{Δt}}_\mathrm n}$
This approach leads to a faster convergence since it responds "faster" to changes in loading or structure (nonlinearities). 
Answer
In RFEM 5 or RFDYNAM Pro  Nonlinear Time History, there are two different methods (also called "solvers" hereafter) available to you for nonlinear, dynamic analyses: the explicit central difference method and the implicit NEWMARK method of mean acceleration (γ = ½ and β = ¼).
In the case of linear systems, the implicit solver is preferable in most cases, because numerically it is absolutely stable, regardless of which time step length is selected. Of course this statement has to be somewhat relativized, given the fact that if the time steps are selected too crudely, substantial inaccuracies in the solution are to be expected. The explicit solver also has only limited stability in linear systems; it becomes stable, when the selected time step is smaller than a specific, critical time step:
$\triangle t\leq\triangle t_{cr}=\frac{T_n}\pi$
In this equation, T_{n} represents the smallest natural vibration period of the FE mesh, which leads to the following statement: The finer the FE mesh gets, the smaller the selected time step should become, in order to ensure numerical stability.
The calculation time of a single time step of the explicit solver is very short, but countless, very fine time steps may just be necessary to get a result at all. For that reason, the implicit NEWMARK solver for dynamic loadings that act over a long period of time, is preferable most of the time. The explicit solver is preferred, when you need to select very fine time steps anyway to get a useful (converging) result. This is the case, for example, in shortterm and erratically variable loadings such as loads from shock or explosion.
In nonlinear systems, both methods are "only" numerically stable, but the implicit NEWMARK solver is still more stable than the central difference method in most cases. For that reason, the same statements as for linear systems apply to nonlinear systems. When the loads are erratically variable and shortterm, the explicit solver is preferable, but in most other cases the NEWMARK solver of mean acceleration is preferred. 
Answer
RF/DYNAM Pro  Equivalent Loads performs a multimodal response spectrum analysis with the export of equivalent loads.
1) The static equivalent loads are calculated and exported to load cases. This happens separately for each mode shape and each direction of excitation.
2) The total earthquake forces can be determined easily for each mode shape.
3) The accidental torsional actions can be considered automatically.
4) The load cases are calculated in the main program RFEM/RSTAB. Possible nonlinearities are taken into account; the calculation parameters of the load cases can be adjusted (for example, the calculation according to the secondorder analysis, deactivation of nonlinearities).
5) The stiffness modifications from the natural vibration cases (NVCs) are not transferred to the load cases automatically.
6) The result combinations are generated individually for each excitation direction (combined modal responses with SRSS or CQC) and for the combination of results from different excitation directions (SRSS, 100%/30% (40%)).
7) The signdependent results are available on the basis of the dominant mode shape, which results in unique RCs.
8) The results can be reproduced step by step.
In RF‑/DYNAM Pro  Forced Vibrations, a multimodal and multipoint response spectrum analysis is performed.
1) A building can be subjected to the excitations by different response spectra at different supports and in different directions.
2) The calculation and superposition are carried out within the RF‑/DYNAM Pro add‑on module. The calculation is linear, nonlinearities are not taken into account. The stiffness modifications from the ESFs are applied.
3) The result combinations of the superimposed results are only exported.

Answer
You always need RF/DYNAM Pro  Natural Vibrations. The additional modules can be purchased depending on your needs. The following additional modules are available: RF/DYNAM Pro  Forced Vibrations and RF/DYNAM Pro  Equivalent Loads.
Contact us
Did you find your question?
If not, contact us via our free email, chat, or forum support, or send us your question via the online form.
First Steps
We provide hints and tips to help you get started with the main programs RFEM and RSTAB.
Wind Simulation & Wind Load Generation
With the standalone program RWIND Simulation, wind flows around simple or complex structures can be simulated by means of a digital wind tunnel.
The generated wind loads acting on these objects can be imported to RFEM or RSTAB.
Your support is by far the best
“Thank you for the valuable information.
I would like to pay a compliment to your support team. I am always impressed how quickly and professionally the questions are answered. I have used a lot of software with a support contract in the field of structural analysis, but your support is by far the best. ”