Using Ratel#
The Ratel library includes support for processing inputs and handling command-line options. Most examples and applications using Ratel will inherit these options.
Command Line Options#
Ratel is controlled via command-line options.
These command line options may be stored in a YML file specified by the runtime option -options_file
.
The following command line options are mandatory:
Option |
Description |
---|---|
|
Path to mesh file in any format supported by PETSc.
Alternatively, a built-in mesh, such as |
|
List of face sets on which to displace by |
Note
This solver can use any mesh format that PETSc’s DMPlex
can read (Exodus, Gmsh, Med, etc.).
Our tests have primarily been using Exodus meshes created using CUBIT; sample meshes used for the example runs suggested here can be found in this repository.
Note that many mesh formats require PETSc to be configured appropriately; e.g., --download-exodusii
for Exodus support.
Consider the specific example of the mesh seen below:

With the sidesets defined in the figure, we provide here an example of a minimal set of command line options:
$ ./bin/ratel-quasistatic -dm_plex_filename [.exo file] -order 4 -E 1e6 -nu 0.3 -bc_clamp 998,999 -bc_clamp_998_translate 0,-0.5,1
In this example, we set the left boundary, face set \(999\), to zero displacement and the right boundary, face set \(998\), to displace \(0\) in the \(x\) direction, \(-0.5\) in the \(y\), and \(1\) in the \(z\).
As an alternative to specifying a mesh with -dm_plex_filename
, the user may use a DMPlex box mesh by specifying -dm_plex_box_faces [int list]
, -dm_plex_box_upper [real list]
, and -dm_plex_box_lower [real list]
.
As an alternative example exploiting -dm_plex_box_faces
, we consider a 4 x 4 x 4
mesh where essential (Drichlet) boundary condition is placed on the top and bottom.
Side 1 is held in place while side 2 is rotated around \(x\)-axis:
$ ./bin/ratel-quasistatic -model elasticity-neo-hookean-initial -E 1 -nu 0.3 -dm_plex_dim 3 -dm_plex_simplex 0 -dm_plex_box_faces 4,4,4 -bc_clamp 1,2 -bc_clamp_2_rotate 0,0,1,0,.05
Note
If the coordinates for a particular side of a mesh are zero along the axis of rotation, it may appear that particular side is clamped zero.
On each boundary node, the rotation magnitude is computed: theta = (c_0 + c_1 * cx) * loadIncrement
where cx = kx * x + ky * y + kz * z
, with kx
, ky
, kz
are normalized values.
The command line options just shown are the minimum requirements to run the application, but additional options may also be set as follows
Option |
Description |
Default value |
---|---|---|
|
CEED resource specifier |
|
|
Filepath to yml file with runtime options for materials with one field |
|
|
Polynomial order of solution basis functions |
|
|
Polynomial order of solution basis functions for all fields |
|
|
Increased quadrature space order; final order given by |
|
|
Order for diagnostic values mesh |
Same value as multigrid fine level order specified via |
|
Geometry order for diagnostic values mesh |
|
|
Filepath to binary file holding restart information and vector |
|
|
List of face sets on which to displace by |
|
|
One or more vectors specifying rigid translation of the face.
Note: If more than one vector is specified, transition times must be provided as |
|
|
One or more rotation axes and rotation polynomial coefficients specifying rigid rotation of the face.
Note: If more than one rotation is specified, transition times must be provided as |
|
|
Transition times between each rigid rotation/translation.
Note: If the first specified time is after |
|
|
Interpolation type between specified rotations/translations ( |
|
|
List of face sets on which to displace by |
|
|
List of face sets on which to set Dirichlet boundary conditions to match a MMS solution |
|
|
List of face sets on which to set Dirichlet boundary conditions to match a MMS solution for a single solution field |
|
|
List of face sets on which to set slip boundary conditions for the components |
|
|
List of indices for the \(k\) components to constrain on the face. The order in which component indices are provided is the same as the order of vector components for |
|
|
One or more vectors specifying rigid translation of the \(k\) constrained components of the face. That is, each translation vector should have length \(k\).
Note: If more than one vector is specified, transition times must be provided as |
Zero vector of length \(k\) |
|
Transition times between each rigid translation.
Note: If the first specified time is after |
|
|
Interpolation type between specified translations ( |
|
|
List of face sets on which to set slip boundary conditions for the components |
|
|
List of face sets on which to set traction boundary conditions with the traction vector(s) |
|
|
Traction vector(s) for face with components given with respect to the global coordinate system.
If more than one vector is specified, transition times must be provided as |
|
|
Transition times between each traction vector.
Note: If the first specified time is after |
|
|
Interpolation type between specified traction vectors ( |
|
|
List of face sets on which to set platen (half-plane) contact boundary conditions. This boundary condition is performed using Nitsche’s method. |
|
|
Specify the center of the platen, with components given with respect to the global coordinate system |
|
|
Specify the exterior normal to the platen, with components given with respect to the global coordinate system.
This vector should point toward the face |
|
|
Distance(s) of the half-plane along the specified normal vector.
In the context of timestepping, the speed of the platen depends on the value of |
|
|
Transition times between each platen distance value, primarily used to control the platen velocity.
Note: If the first specified time is after |
|
|
Interpolation type between specified distance values ( |
|
|
Nitsche’s method penalty parameter, larger values result in less erroneous penetration. Generally, should be ~100 times the Young’s modulus. |
|
|
Coefficient of friction, or |
|
|
List of face sets on which to set pressure boundary conditions. |
|
|
Specify the pressure. |
|
|
Material model to use ( |
|
|
Forcing term option ( |
|
|
Forcing vector |
|
|
PC type for linear solver |
|
|
P-Multigrid coarsening to use ( |
|
|
Array of orders for each multigrid level, in ascending order; fine grid order specified by |
|
|
Polynomial order of coarse grid basis functions for materials with one field.
This is only used with |
|
|
List of face sets on which to compute surface force |
|
|
Increased quadrature space order for cell-to-face surface force computation; final order given by |
|
|
Expected strain energy, for testing |
|
|
Expected max displacement in a particular direction ( |
|
|
Expected surface force on face |
|
|
Expected surface forces on face |
|
|
Expected centroid of face |
|
|
Expected centroid of face |
|
|
Output final solution for viewing, ASCII format to STDOUT is used if no viewer is passed |
|
|
Output computed strain energy on each time step |
|
|
Output final solution for viewing, ASCII format to STDOUT is used if no viewer is passed |
|
|
Output centroid displacements and accurate surface forces computed using the volumetric residual operator (reaction force) for faces given by |
|
|
Output centroid displacements and approximate surface forces computed using cell-to-face quadrature for faces given by |
|
|
Output binary file with solution checkpoints for continuation. Note: Binary viewer and extension are always used. |
|
|
Number of time steps between checkpoint output |
|
|
Output binary file with final solution checkpoint.
Note: Automatic with |
|
|
View PETSc |
|
|
View PETSc |
|
|
View PETSc performance log |
|
|
Deprecated: Use |
|
|
View comprehensive information about run-time options |
To verify the convergence of the linear elasticity formulation on a given mesh with the method of manufactured solutions, run:
$ ./bin/ratel-quasistatic -dm_plex_filename [mesh] -order [order] -model elasticity-linear -nu [nu] -E [E] -forcing mms
This option attempts to recover a known solution from an analytically computed forcing term.
Material Properties#
Each material model has properties that need to be specified. All properties are mandatory.
Option |
Description |
Model |
---|---|---|
|
Young’s modulus, \(E > 0\) |
Neo-Hookean |
|
Poisson’s ratio, \(\nu < 0.5\) |
Neo-Hookean or Mooney-Rivlin |
|
Poisson’s ratio for multigrid smoothers, \(\nu < 0.5\) |
Neo-Hookean or Mooney-Rivlin |
|
Mooney-Rivlin material constant, \(\mu_1 > 0\), |
Mooney-Rivlin |
|
Mooney-Rivlin material constant, \(\mu_2 > 0\) |
Mooney-Rivlin |
|
Initial yield stress threshold, \(\sigma_0 > 0\) |
Linear Plasticity |
|
Isotropic hardening parameter, \(A > 0\) |
Linear Plasticity |
Multiple Materials#
Ratel supports the use of solving with different material models defined for different segments of the mesh.
This feature requires additional runtime flags as well as some modifications to existing flags.
Different materials should be specified over labeled volumes of the mesh; an example of the header of a Gmsh mesh (provided in examples/meshes/materials_2.msh
) with two materials (“rod” and “binder”) is shown below:
$ head examples/meshes/materials_2.msh
$MeshFormat
4.1 0 8
$EndMeshFormat
$PhysicalNames
4
2 1 "start"
2 2 "end"
3 3 "rod"
3 4 "binder"
$EndPhysicalNames
In this example, the ID value of the “rod” and “binder” volumes are 3 and 4, respectively.
In order to tell Ratel to treat these volumes as different materials, we use -material rod,binder
to provide label names for our specified materials (Note: these names do not have to match the names in the Gmsh mesh).
These label names will be used as prefixes (as -{material name}_
) to specify other aspects for each material at runtime.
We also specify, for each material, which domain label values to use with -rod_label_value 3 -binder_label_value 4
.
To define material parameters such as \(E\) and \(\nu\), we now use -binder_E 2.0 -binder_nu 0.4
.
An example set of command line options for the setting rods and binder materials is given below:
$ ./bin/ratel-quasistatic -material rod,binder -rod_model elasticity-mooney-rivlin-initial -rod_mu_1 0.5 -rod_mu_2 0.5 -rod_nu 0.4 -binder_label_value 3 -binder_model elasticity-neo-hookean-initial -binder_E 2.0 -binder_nu 0.4 -binder_label_value 4
A complete list of command line options for specifying multiple materials is given below in the next table:
Option |
Description |
Default value |
---|---|---|
|
List of names to use as labels for each material. |
|
|
Material to use ( |
|
|
Domain label specifying the type of volume to use for specifying materials. Optional. |
|
|
Domain value specifying the volume to use for a given material. |
|
|
Young’s modulus, \(E > 0\) |
|
|
Poisson’s ratio, \(\nu < 0.5\) |
|
|
Poisson’s ratio for multigrid smoothers, \(\nu < 0.5\) |
An example of specifying a two material quasistatic solve with YAML is provided in examples/ex02-quasistatic-elasticity-multi-material.yml
.
Algebraic Solvers#
The examples are configured to use the following Newton-Krylov-Multigrid method by default.
Newton-type methods for the nonlinear solve, with the hyperelasticity models globalized using load increments.
Preconditioned conjugate gradients to solve the symmetric positive definite linear systems arising at each Newton step.
Preconditioning via \(p\)-version multigrid coarsening to linear elements, with algebraic multigrid (PETSc’s
GAMG
) for the coarse solve. The default smoother uses degree 3 Chebyshev with Jacobi preconditioning. (Lower degree is often faster, albeit less robust; try-mg_levels_ksp_max_it 2
, for example.) Application of the linear operators for all levels with order \(p > 1\) is performed matrix-free using analytic Newton linearization, while the lowest order \(p = 1\) operators are assembled explicitly (using coloring at present).
Many related solvers can be implemented by composing PETSc command-line options.
For example, to use Hypre’s BoomerAMG for the coarse solve (using the assembled linear elements), one would use -mg_coarse_pc_type hypre
.
Run with -help
to see (many!) available command-line options related to algebraic solvers.
Nondimensionalization#
Quantities such as the Young’s modulus vary over many orders of magnitude, and thus can lead to poorly scaled equations. One can nondimensionalize the model by choosing an alternate system of units, such that displacements and residuals are of reasonable scales.
Option |
Description |
Default value |
---|---|---|
|
1 meter in scaled length units |
|
|
1 second in scaled time units |
|
|
1 kilogram in scaled mass units |
|
For example, consider a problem involving metals subject to gravity.
Quantity |
Typical value in SI units |
---|---|
Displacement, \(\bm u\) |
\(1 \,\mathrm{cm} = 10^{-2} \,\mathrm m\) |
Young’s modulus, \(E\) |
\(10^{11} \,\mathrm{Pa} = 10^{11} \,\mathrm{kg}\, \mathrm{m}^{-1}\, \mathrm s^{-2}\) |
Body force (gravity) on volume, \(\int \rho \bm g\) |
\(5 \cdot 10^4 \,\mathrm{kg}\, \mathrm m^{-2} \, \mathrm s^{-2} \cdot (\text{volume} \, \mathrm m^3)\) |
One can choose units of displacement independently (e.g., -units_meter 100
to measure displacement in centimeters), but \(E\) and \(\int \rho \bm g\) have the same dependence on mass and time, so cannot both be made of order 1.
This reflects the fact that both quantities are not equally significant for a given displacement size; the relative significance of gravity increases as the domain size grows.
Diagnostic Quantities#
Diagnostic quantities for viewing are provided when the command line option for visualization output, -view_diagnostic_quantities viewer:filename.extension
is used.
The diagnostic quantities include displacement in the \(x\) direction, displacement in the \(y\) direction, displacement in the \(z\) direction, pressure, \(\operatorname{trace} \bm{E}\), \(\operatorname{trace} \bm{E}^2\), \( J \), and strain energy density \(\psi\).
The table below summarizes the formulations of each of these quantities for each material type.
Quantity |
Linear elasticity |
Neo-Hookean hyperelasticity |
---|---|---|
Cauchy stress tensor |
\(\bm{\sigma}\) |
\(\bm{\sigma} = \bm{F} \bm{S} \bm{F}^T / J \) |
Pressure |
\(\lambda \operatorname{trace} \bm{\epsilon}\) |
\(\frac{\lambda}{2J} \left(J^2 - 1\right) \) |
Volumetric strain |
\(\operatorname{trace} \bm{\epsilon}\) |
\(\operatorname{trace} \bm{E}\) |
\(\operatorname{trace} \bm{E}^2\) |
\(\operatorname{trace} \bm{\epsilon}^2\) |
\(\operatorname{trace} \bm{E}^2\) |
\( J \) |
\(1 + \operatorname{trace} \bm{\epsilon}\) |
\( J \) |
Strain energy density |
\(\frac{\lambda}{2} (\operatorname{trace} \bm{\epsilon})^2 + \mu \bm{\epsilon} : \bm{\epsilon}\) |
\(\frac{\lambda}{4}\left(J^2 - 1 - 2 \log J \right) + \mu \operatorname{trace} \bm{E} - \mu \log J\) |
von Mises stress |
\(\sqrt{\frac 3 2 \bm{\hat \sigma} \tcolon \bm{\hat \sigma}}\) |
\(\sqrt{\frac 3 2 \bm{\hat \sigma} \tcolon \bm{\hat \sigma}}\) |
The von Mises stress uses the deviatoric part \(\bm{\hat\sigma} = \bm{\sigma} - \frac 1 3 \trace \bm{\sigma}\) of the Cauchy stress \(\bm{\sigma}\). The integrated strain energy \(\Psi = \int_{\Omega_0} \psi\) is also computed and printed upon completion of a solve.