This is the information needed for the analysis and not related to the geometry.
|
|
||||||
|
|
Mesh units are the units in which are represented the coordinates of the geometry and mesh. Results units are the units used to represent the results of the analysis.
Mesh units can be: meter (m), centimeter (cm) or millimeter (mm)
Results units can be expressed as:
Displacements are in m
Velocities are in m/s
Accelerations in m/s^2
Strengths are in N/m or N·m/m
Stresses are in Pa= N/m2
Displacements are in mm
Velocities are in mm/s
Accelerations in mm/s^2
Strengths are in N/mm or N·mm/mm
Stresses are in N/mm2
Displacements are in cm
Velocities are in cm/s
Accelerations in cm/s^2
Strengths are in Kp/cm or Kp·cm/cm
Stresses are in Kp/cm2
Displacements are in m
Velocities are in m/s
Accelerations in m/s^2
Strengths are in kN/m or kN·m/m (kN=103 N)
Stresses are in Mpa=106 Pa
Note that the units in this last system does not form a compatible system.
The three components of the gravity define a vector, which will be normalized inside the program , and represents the direction of the gravity if the self-weight is considered.
Beam Res granularity means the number of subdivisions that will have every beam to represent the results. More subdivisions give more quality in the results visualization and more disk space. This option does not modify the precision of the result, only its visualization.
Shell res axes permits to choose if the strengths results will be displayed in local axes , in main axes or in both . Local axes are the ones defined in the properties section. Main axes will be defined later. If it is not necessary to save disk space, choose both .
Output shell stresses If chosen, the stresses and Von Misses in both, the face up and the face down of the shell are calculated.
Output_beams_Maximums When there are more than one loadcase, it is possible to output a special loadcase containing the maximums for beams. Option Automatic , outputs it only if there are steel sections. Option Always , output it if there are more than one loadcase.
Shell internal 6-noded elem If chosen, mesh generated as 3-noded triangle elements will be internally calculated as 6-noded triangles. It gives more precision in the results and needs more computer time. It should be always used except when strengths in the shell plane are dominant. In this last case, both options are feasible.
Shell smooth res If chosen, rambshell will smooth the strength results where possible. The results of the calculation are strengths in the interior of every element that are discontinuous from one element to another. Smoothing means to approximate other values of the strengths so as they are continuous from one element to another. This can only be made if the geometry is smooth by itself from one element to another.
Smooth per material : (option only available for solids). When mixing two materials very different, like steel and concrete, the stresses are not continuus between materials. Then, it is necessary to set this option in order to see the stresses jump in the two materials boundary.
Problem type : Normally, this option should be set to Beams and shells. If the problem to analyze has only elements in one plane and it can be considered as a plane strain, plane stress or a plate problem, select one of these options. In these cases, the input of the data is the same than for the general analysis but the problem to solve is much faster. So, it saves a lot of computing time.
Consider Beam P-Delta : if this option is set, the beam P-delta method is applied in order to calculate second order effects for columns.
Be careful because one of the effects in a bad designed structure is that it will not be possible to obtain a solution. The recommended way of working is to calculate first in first order, and after with second order. If the strengths increment more than a certain value (20%-30%), a redesign of the structure is advised.
Analysis : This option select the type of analysis to be perform. Rambshell can perform the following analyisis:
- Linear Static
- Linear Dynamic
- Non-Linear Static
- Non-Linear Dynamic
If the Analysis Type option is set in the Linear Dynamic, and the bottom Analysis Preferences is pressed the following data must be indicated
- Dynamic Analysis Type: There are tree possible types of dynamic analysis:
1-) Modal Analysis
2-) Direct Integration
3-) Spectrum Analysis.
1-) Modal Analysis
![]() |
|
If chosen, the following options appear:
Number of modes: Indicates the number of modes to be considered in the vibrations analysis.
DeltaT: Indicate the step of time to be considered in the dynamic analysis.
Number of steps: Indicates the total number of steps considered in the analysis. The total physical time will be DeltaT x Number_of_steps.
Matrix Storage: Indicates the way to be storage the dynamical matrix. There are two possibilities: Lumped and Consistent. A lumped matrix storage means that the masses are concentrated in the nodes and then the mass matrix are reduced to vector. A consistent matrix storage means that the masses are consider consistently with the finite element approach and then the mass matrix is storage completely.
Damping Type: Indicates the way that the damping is considered. There are two possibilities: Modal Damping and Rayleigh Damping. In the modal damping option the damping is taking in account in the equations of motions of each mode without compute any Damping Matrix, with this option is necessary to input the damping ratio. In the Rayleigh damping option is computed a Damping Matrix proportional to the stiffness and mass Matrices, with this option is necessary to input the coefficients Alpha_M and Alpha_K.
Initial Conditions: Indicates the initial conditions in displacements for the dynamical analysis. The initial displacements considered are that obtain in static analysis in Combined Load case 1.
2-) Direct Integration
![]() |
|
If chosen, the following options appear:
DeltaT: Indicates the step of time to be considered in the dynamic analysis.
Number of steps: Indicates the total number of steps considered in the analysis. The total physical time will be DeltaT x Number_of_steps.
Gamma: Parameter for the direct integration method.
Beta: Parameter for the direct integration method.
Matrix Storage: Indicates the way to be storage the dynamical matrix. There are two possibilities: Lumped and Consistent. A lumped matrix storage means that the masses are concentrated in the nodes and then the mass matrix are reduced to vector. A consistent matrix storage means that the masses are consider consistently with the finite element approach and then the mass matrix is storage completely.
Damping Type: Indicates the way that the damping is considered. For Direct Integrations approach only Rayleigh Damping can be used. with this option is necessary to input the coefficients Alpha_M and Alpha_K.
Initial Conditions: Indicates the initial conditions in displacements for the dynamical analysis. The initial displacements considered are that obtain in static analysis in Combined Load case 1.
3-) Spectrum Analysis
![]() |
|
If chosen, the following options appear:
Number of modes: Indicates the number of modes to be considered in the vibrations analysis.
Matrix Storage: Indicates the way to be storage the dynamical matrix. There are two possibilities: Lumped and Consistent. A lumped matrix storage means that the masses are concentrated in the nodes and then the mass matrix are reduced to vector. A consistent matrix storage means that the masses are consider consistently with the finite element approach and then the mass matrix is storage completely.
Damping Type: Indicates the way that the damping is considered. There are two possibilities: Modal Damping and Rayleigh Damping. In the modal damping option the damping is taking in account in the equations of motions of each mode without compute any Damping Matrix, with this option is necessary to input the Damping ratio. In the Rayleigh damping option is computed a Damping Matrix proportional to the stiffness and mass Matrices, with this option is necessary to input the coefficients Alpha_M and Alpha_K.
Spectrum Analysis type: Indicates the type of Spectrum Analysis to perform. There are two possibilities:
Seismic Codes: Is possible to perform the spectrum analysis establish in the NCSE-94 Spanish regulation.
User defined spectrum: The user have the possibility to input his own spectrum of accelerations.
|
|
If the Analysis Type option is set in the Linear Dynamic, and the bottom Analysis Preferences is pressed the following data must be indicated
![]() |
|
Delta Fac indicates the incremental factor for the load.
Num inc indicates the number of parts that the total load is divided
Automatic inc indicates if an automatic incrementation procedure is required
Control indicates the type of load control required for the analysis. Ramseries can perform a Load Control, Displacement Control and Arc-Length control
Conv. tolerance static represents the convergence value for the Non-Linear Static analysis.
Iteration type indicates when the structural stiffness matrix is recalculated. Ramseries can perform a recalculation in each iteration of each load step (Full_N-R) or a recalculation in the first iteration of each load step (Modified_N-R).
Max iter indicates the maximun number of iteration allowed in each load step
Line-Searc h indicates if the line-search method is required
Auto-ARC -switch indicates if an automatic switch to the Arc-Length Control is required.
If the Automatic inc option is set, the following data must be indicated
![]() |
|
Num Iter d indicates the number of iteration desired in each load step.
DeltaP max indicates the maximal load increment allowed.
DeltaP min indicates the minimal load increment allowed.
If the Line-Search option is chosen, the following data must be indicated
![]() |
|
LS-loops define the maxim number of Line-Search loops.
LS-toler define tolerance ratio desidered .
LS-min define the maximal step-length of Line-Search.
LS-max define the minimal step-length of Line-Search.
Amp-max define the maximal amplitude of any step.
If the Line-Search option is chosen, the following datum must be indicated
![]() |
|
C Stif indicate the desired current stiffness parameter for swithching.
If the Analysis Type option is set in the Non-Linear Dynamic, and the bottom Analysis Preferences is pressed the following data must be indicated
![]() |
|
Integration method indicates the algorithm of temporal integration to be performed in the Non-Linear Dynamics analysis. Ramseries can perform Implicit or Explicit temporal integration method.
T 0 indicates the initial time for the dynamic analysis. In general this value is set to zero.
DeltaT_variation indicates the time step variation for certain number of step. This options is very useful when different time step are required in the analysis.
Matrix-storage choose the type of storage for the Mass and Damping Matrix. This storage can be in a Lumped diagonal vector or in a Consistent matrix.
Initial Condition indicate which type of intial conditions are required. The intial condition can defined manually for the users (User_Defined) or can be assigned like initial conditions the values obtained in the static linear elastic analysis performed in the Combinated Load Case 1 (Comb._Load_1)
![]() |
|
Gamma and Beta represent parameters for the Newmark method of temporal integration.
![]() |
|
Alpha M represents the coefficient of the Mass Matrix in the Rayleigh Damping
Alpha K represents coefficient of the Damping Matrix in the Rayleigh Damping
![]() |
|
Conv. tolerance dynamic represents the convergence tolerance factor for the Non-Linear-Dynamic analysis.
Iteration-type indicates if the full,modified o intial Newton Raphson method is chosen.
Max-iter defines the maximun number of iterations.