RamSeries manual


Problem data

This is the information needed for the analysis and not related to the geometry.

Units

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:

¨       N-m-kg where:

o        Displacements are in m

o        Velocities are in m/s

o        Accelerations in m/s^2

o        Strengths are in N/m or N·m/m

o        Stresses are in Pa= N/m2

¨       N-mm-kg where:

o        Displacements are in mm

o        Velocities are in mm/s

o        Accelerations in mm/s^2

o        Strengths are in N/mm or N·mm/mm

o        Stresses are in N/mm2

¨       Kp-cm where:

o        Displacements are in cm

o        Velocities are in cm/s

o        Accelerations in cm/s^2

o        Strengths are in Kp/cm or Kp·cm/cm

o        Stresses are in Kp/cm2

¨       KN,m,Mpa where:

o        Displacements are in m

o        Velocities are in m/s

o        Accelerations in m/s^2

o        Strengths are in kN/m or kN·m/m (kN=103 N)

o        Stresses are in Mpa=106 Pa

Note that the units in this last system does not form a compatible system.

Gravity

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.

Results

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.

Analysis

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 to do Static and Dynamic analysis. If it is set in the Dynamic option appear the following option related with the dynamic analysis:

- 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: Indicate 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: Indicate the total number of steps considered in the analysis. The total physical time will be DeltaT x Number_of_steps.

·         Matrix Storage: Indicate 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: Indicate 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: Indicate 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: Indicate the step of time to be considered in the dynamic analysis.

·         Number of steps: Indicate 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: Indicate 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: Indicate 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: Indicate 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: Indicate the number of modes to be considered in the vibrations analysis.

·         Matrix Storage: Indicate 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: Indicate 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: Indicate 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.