Skip to main content
`Ctrl`+`K`

# Solution Cases

Example files on this page

- eigen input file — Salinas_rtest/training/exampleproblem/eigen/fixture/eigen.inp

- Fixture Mesh — Salinas_rtest/training/exampleproblem/static/fixture/fixture.exo

- modal transient simulation — Salinas_rtest/training/exampleproblem/transient/modaltrans/fixtureB/mtrans.inp

- modalfrf input file — Salinas_rtest/training/exampleproblem/frf/modal/fixture/mfrf.inp

- modalranvib input file — Salinas_rtest/training/exampleproblem/randomvib/fixture/rvib.inp

- statics input file — Salinas_rtest/training/exampleproblem/static/fixture/static.inp

- transient input file — Salinas_rtest/training/exampleproblem/transient/displacement/fixture/dtrans.inp

# 1. Solution Cases

Sierra/SD supports different analysis types via solution cases. This section covers simple examples of several of the most common of these solution cases. Each of these input decks use the same “Fixture” mesh shown in Figure 1.1.

Figure 1.1 Fixture Mesh

The sections of a Sierra/SD input file are described in the Sierra SD Users’ Guide. An input file has several common sections: solution, file (Exodus mesh), load(s), outputs, echo, block (one per element block in the input Exodus file) and material (one per unique material).

The statics input file has the common sections, and three optional sections: parameters, boundary and GDSW. The parameter Wtmass, typically \(1/(32.2 ft/s^2\) \(12 in/ft)\), is used so that for example densities may be specified in units of \(lbs/in^3\), as described in the Users’ Guide. Boundary conditions on a side set, or in this case a node set, are specified in the boundary section. The GDSW section indicates that the threshold on the relative residual norm be decreased from the default 1.e-6 if using the GDSW linear solver.

The eigen input file requests that the twelve lowest frequency modes be computed. The eigen norm parameter indicates that the mode shapes will be normalized in a way that is convenient for visualization. The default normalization uses the mass matrix. Here `solver_tol` has been further reduced to \(1.e-10\).

The transient input file uses the default Newmark method and has the total simulation time of 1/100 seconds. The load is specified by a tabulated Haversine pulse. The history section indicates that the output quantities at each time step and at the specified node sets only will be written to a different Exodus output file with the suffix h. In this case the history file name is `fixture-out.h`. The history file is \(20,000\) times smaller than the ordinary output file. Finally, the restart option in the solution section means that the file fixture-out.rslt_trans will be written. It is possible to restart the simulation using this restart file, as described in the Users’ Guide.

In a modal transient simulation, the transient problem is projected onto the subspace spanned by the mode shapes of a user specified number of the lowest frequency modes. Modal transient simulations are typically much faster than direct transient analyses. The `transient` keyword has been replaced by the `modaltransient` keyword. Also, a single input file is used for both the initial eigenvalue problem (\(20\) modes), and the following modal transient solution. This is called a multicase solution. Another difference is that the plural `loads` section has been replaced by a numbered `load` block to define a load that applies to the transient solution, but not to the eigen solution.

Returning to the first solution case in the modal transient simulation, the eigenvalue problem, a shift is set to \(-1e+6\). Here the first eigenvalue is \(1e+8\). The eigenvalue problem is solved more efficiently and accurately if the shift is approximately \(-1\) times the lowest nonzero eigenvalue (flexible mode).

The modalfrf input file concerns the frequency response function. The frequency response function is used for example to confirm engineering assumptions about the frequency content of the accelerations.

\[ \hat{u}(\omega)=(K + i \omega C - \omega^2 M)^{-1}\hat{f}(\omega), i=\sqrt{-1}. \]

Modal frequency response refers to using the mode shapes to diagonalize the transfer function. A linear solver is not used to evaluate the transfer function, but is used in solving the eigenvalue problem. The function here describes the frequency dependent load, the Fourier transform of the temporal load. The `damping` section supplies the coefficient for mode proportional damping, \(C = \gamma M\). The frequency block sets the spatial location and frequency range of the load.

In the modal frequency response problem note that there is both a history section and a frequency section. The input file is for a multicase simulation. The history file section applies to the solution of the eigenvalue problem, and is ignored during the solution of the frequency response problem. The frequency response section is ignored during the solution of the eigenvalue problem, and applies only to the frequency response problem.

The modalranvib input file calculates the response of the to random vibration inputs. This solution has similarities to the modalfrf solution case and additionally requires a frequency dependent load definition. The outputs of this analysis are statistical properties of acceleration, velocity, displacement, and stress to the random vibration inputs. This case is covered in more detail in Modal Random Vibration.