(using)=
# Using Ratel
The Ratel library includes support for processing inputs and handling commandline options.
Most examples and applications using Ratel will inherit these options.
## Command Line Options
Ratel is controlled via commandline 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:
:::{listtable} Mandatory Runtime Options
:headerrows: 1
:widths: 3 7
*  Option
 Description
*  `dm_plex_filename [filename]`
 Path to mesh file in any format supported by PETSc.
Alternatively, a builtin mesh, such as `dm_plex_box` may be specified.
*  `bc_clamp [int list]`
 List of face sets on which to displace by `bc_clamp_[facenumber]_translate [x,y,z,...]` and/or `bc_clamp_[facenumber]_rotate [rx,ry,rz,c_0,c_1]`.
Note: The default for a clamped face is zero displacement.
All displacement is with respect to the initial configuration.
At least one fixed boundary is required to prevent a singular system.
:::
:::{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., `downloadexodusii` for Exodus support.
:::
Consider the specific example of the mesh seen below:
```{image} https://github.com/jeremylt/ceedSampleMeshes/raw/master/cylinderDiagram.png
```
With the sidesets defined in the figure, we provide here an example of a minimal set of command line options:
```console
$ ./bin/ratelquasistatic 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 {code}`dm_plex_filename`, the user may use a DMPlex box mesh by specifying {code}`dm_plex_box_faces [int list]`, {code}`dm_plex_box_upper [real list]`, and {code}`dm_plex_box_lower [real list]`.
As an alternative example exploiting {code}`dm_plex_box_faces`, we consider a {code}`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:
```console
$ ./bin/ratelquasistatic model elasticityneohookeaninitial 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: {code}`theta = (c_0 + c_1 * cx) * loadIncrement` where {code}`cx = kx * x + ky * y + kz * z`, with {code}`kx`, {code}`ky`, {code}`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
:::{listtable} Additional Runtime Options
:headerrows: 1
:widths: 25 50 25
*  Option
 Description
 Default value
*  `ceed [string]`
 CEED resource specifier
 `/cpu/self`
*  `options_file [filename]`
 Filepath to yml file with runtime options for materials with one field
 `/path/to/my.yml`
*  `method [fem  mpm]`
 Numerical method used to run simulations, either Finite Element Method (`fem`) or Material Point Method (`mpm`). See `mpm_*` for MPM specific options.
 `fem`
*  `mpm_num_points [int]`
 Total number of material points, divided evenly between cells in the domain. Only used if `mpm_num_points_per_cell` is not provided.
 `1728`
*  `mpm_num_points_per_cell [int]`
 Number of material points per cell, rounded up to the nearest cube. If not provided, `mpm_num_points` is used.

*  `mpm_point_location_type [gauss  uniform  cell_random]`
 Initial position of material points percell.
If `gauss`, uses the Gauss quadrature points.
If `uniform`, points are uniformly spaced within the cell. The distance between points across cell boundaries is also uniform.
If `cell_random`, points are placed randomly with each cell. Note that each cell will still contain the same number of points.
 `uniform`
*  `order [int]`
 Polynomial order of solution basis functions
 `3`
*  `orders [int list]`
 Polynomial order of solution basis functions for all fields
 `3`
*  `q_extra [int]`
 Increased quadrature space order; final order given by `order[0] + q_extra`
 `0`
*  `diagnostic_order [int]`
 Order for diagnostic values mesh
 Same value as multigrid fine level order specified via `order`
*  `diagnostic_geometry_order [int]`
 Geometry order for diagnostic values mesh

*  `continue_file [filename]`
 Filepath to binary file holding restart information and vector

*  `bc_clamp [int list]`
 List of face sets on which to displace by `bc_clamp_[facenumber]_translate [x,y,z,...][,x2,y2,z2,...]` and/or `bc_clamp_[facenumber]_rotate [rx,ry,rz,c_0,c_1][,r2x,r2y,r2z,c2_0,c2_1,...]`.
If more than one translation and/or rotation is specified, transition times must be provided as `bc_clamp_[facenumber]_times [t1,t2,...]`.
If `t1 > 0`, a node with zero translation and rotation will be added implicitly at time `0`.
Note: The default for a clamped face is zero displacement.

*  `bc_clamp_[facenumber]_translate [x,y,z,...][,x2,y2,z2,...]`
 One or more vectors specifying rigid translation of the face.
Note: If more than one vector is specified, transition times must be provided as `bc_clamp_[facenumber]_times [t1,t2,...]`.
Note: If the constrained field has more than 3 components, such as a damage component, later components may be translated but not rotated.
 `0,0,0`
*  `bc_clamp_[facenumber]_rotate [rx,ry,rz,c_0,c_1][,r2x,r2y,r2z,c2_0,c2_1,...]`
 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 `bc_clamp_[facenumber]_times [t1,t2,...]`.
Note: If the constrained field has more than 3 components, such as a damage component, later components may be translated but not rotated.
 `0,0,0,0,0`
*  `bc_clamp_[facenumber]_times [t1,t2,...]`
 Transition times between each rigid rotation/translation.
Note: If the first specified time is after `0`, a rotation and translation of `0,0,0,0,0` and `0,0,0`, respectively, will be added with time `0` in order to start from an undeformed configuration.
 `1`
*  `bc_clamp_[facenumber]_interpolation`
 Interpolation type between specified rotations/translations (`none` or `linear`).
 `linear`
*  `bc_clamp_field_[fieldnumber] [int list]`
 List of face sets on which to displace by `bc_clamp_field_[fieldnumber]_face_[facenumber]_translate [x,y,z]` and/or `bc_clamp_field_[fieldnumber]_face_[facenumber]_rotate [rx,ry,rz,c_0,c_1]` for a single solution field.
Also supports lists of rotations or translations, see details in `bc_clamp` above.
Note: The default for a clamped face is zero displacement.

*  `bc_clamp_[fieldname] [int list]`
 List of face sets on which to displace by `bc_clamp_[fieldname]_face_[facenumber]_translate [x,y,z,...]` and/or `bc_clamp_[fieldname]_face_[facenumber]_rotate [rx,ry,rz,c_0,c_1]` for a single solution field.
Also supports lists of rotations or translations, see details in `bc_clamp` above.
Note: The default for a clamped face is zero displacement.

*  `bc_mms [int list]`
 List of face sets on which to set Dirichlet boundary conditions to match a MMS solution

*  `bc_mms_field_[fieldnumber] [int list]`
 List of face sets on which to set Dirichlet boundary conditions to match a MMS solution for a single solution field

*  `bc_mms_[fieldname] [int list]`
 List of face sets on which to set Dirichlet boundary conditions to match a MMS solution for a single solution field

*  `bc_slip [int list]`
 List of face sets on which to set slip boundary conditions for the components `bc_slip_[facenumber]_components [int list]`

*  `bc_slip_[facenumber]_components [int list]`
 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 `bc_slip_[facenumber]_translate`.

*  `bc_slip_[facenumber]_translate [c1,...,ck][c1_2,...,ck_2,...,c1_n,...,ck_n]`
 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 `bc_slip_[facenumber]_times [t1,t2,...]`.
 Zero vector of length $k$
*  `bc_slip_[facenumber]_times [t1,t2,...]`
 Transition times between each rigid translation.
Note: If the first specified time is after `0`, a translation of `0,0,0` will be implicitly added with time `0` in order to start from an undeformed configuration.
 `1`
*  `bc_slip_[facenumber]_interpolation`
 Interpolation type between specified translations (`none` or `linear`).
 `linear`
*  `bc_slip_field_[fieldnumber] [int list]`
 List of face sets on which to set slip boundary conditions for the components `bc_slip_field_[fieldnumber]_face_[facenumber]_components [int list]` for a single solution field.
Also supports lists of translations, see details in `bc_slip` above.

*  `bc_slip_[fieldname] [int list]`
 List of face sets on which to set slip boundary conditions for the components `bc_slip_[fieldname]_face_[facenumber]_components [int list]` for a single solution field.
Also supports lists of translations, see details in `bc_slip` above.

*  `bc_traction [int list]`
 List of face sets on which to set traction boundary conditions with the traction vector(s) `bc_traction_[facenumber] [tx,ty,tz][,t2x,t2y,t2z,...]`.

*  `bc_traction_[facenumber] [tx,ty,tz][,t2x,t2y,t2z,...]`
 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 `bc_traction_[facenumber]_times [t1,t2,...]`.

*  `bc_traction_[facenumber]_times [t1,t2,...]`
 Transition times between each traction vector.
Note: If the first specified time is after `0`, a traction vector of `0,0,0` will be added with time `0` in order to start from an undeformed configuration.
By default, linearly applies traction from `t = 0` to `t = 1`
 `1`
*  `bc_traction_[facenumber]_interpolation`
 Interpolation type between specified traction vectors (`none` or `linear`).
 `linear`
*  `bc_platen [string list]`
 List of labels for each platen (halfplane) contact boundary condition to apply. Examples: "top,bottom" or "1,2"
This boundary condition is performed using Nitsche's method.

*  `bc_platen_[platen_name]_type [nitschepenalty]`
 Solver method to use for platen boundary, either `nitsche` for Nitsche's method or `penalty` for penalty method.
 `nitsche`
*  `bc_platen_[platen_name]_label_value`
 Value of `DMPlex` label to apply the platen to (such as the face label). If `platen_name` is a string then the label value must be provided.
 `platen_name` if `platen_name` is an integer.
*  `bc_platen_[platen_name]_center [cx,cy,cz]`
 Specify the center of the platen, with components given with respect to the global coordinate system

*  `bc_platen_[platen_name]_normal [nx,ny,nz]`
 Specify the exterior normal to the platen, with components given with respect to the global coordinate system.
This vector should point toward the face `[facenumber]`.

*  `bc_platen_[platen_name]_distance [dist][,dist2,dist3,...]`
 Distance(s) of the halfplane along the specified normal vector.
In the context of timestepping, the speed of the platen depends on the value of `bc_platen_[platen_name]_interpolation`.
If more than one distance is specified, transition times must be provided as `bc_platen_[platen_name]_times [t1,t2,...]`.
 `0.0`
*  `bc_platen_[platen_name]_times [t1,t2,...]`
 Transition times between each platen distance value, primarily used to control the platen velocity.
Note: If the first specified time is after `0`, a distance of `0` will be added implicitly with time `0` in order to start from an undeformed configuration.
Note: If a single distance is provided, the time value defaults to `1`; i.e., the platen will move the prescribed distance in `1` time unit.
 `1`
*  `bc_platen_[platen_name]_interpolation`
 Interpolation type between specified distance values (`none` or `linear`).
Note: `none` results in piecewiseconstant displacement while `linear` results in piecewiselinear displacement and piecewiseconstant velocity.
 `linear`
*  `bc_platen_[platen_name]_gamma [real]`
 Nitsche's method penalty parameter, larger values result in less erroneous penetration. Generally, should be ~100 times the Young's modulus.
 `1.0`
*  `bc_platen_[platen_name]_friction_type [nonecoulombthrelfall]`
 Specify the type of friction to use, see [Friction Models](modeling/governingequations/friction) for details on available models.
 `none`
*  `bc_platen_[platen_name]_friction_kinetic [nonnegative real]`
 Kinetic (sliding) coefficient of friction $\mu_k$, unitless.
 `0.1`
*  `bc_platen_[platen_name]_friction_static [nonnegative real]`
 Static (slipping) coefficient of friction $\mu_s > \mu_k$, unitless. Not currently used.
 `0.15`
*  `bc_platen_[platen_name]_friction_viscous [nonnegative real]`
 Viscous damping coefficient $F_v$, units of $\frac{\mathrm{N}\cdot\mathrm{s}}{\mathrm{m}}$.
 `0.0`
*  `bc_platen_[platen_name]_friction_tolerance_velocity [positive real]`
 Tolerance velocity $v_0$ at which full frictional slipping is permitted, units of $\frac{\mathrm{m}}{\mathrm{s}^2}$. Only used by Threlfall friction model.
 `0.05`
*  `bc_platen_[platen_name]_f [nonnegative real]`
 Deprecated: Use `bc_platen_[platen_name]_friction_type coulomb` and `bc_platen_[platen_name]_friction_kinetic [nonnegative real]` for the same functionality.
 `0`
*  `bc_pressure [int list]`
 List of face sets on which to set pressure boundary conditions.

*  `bc_pressure_[facenumber] [real t1p][,t2p,t3p,...]`
 Pressure value(s) for face with components given with respect to the global coordinate system.
If more than one pressure is specified, transition times must be provided as `bc_pressure_[facenumber]_times [t1,t2,...]`.

*  `bc_pressure_[facenumber]_times [t1,t2,...]`
 Transition times between each pressure value.
Note: If the first specified time is after `0`, a pressure vector of `0` will be added with time `0` in order to start from an undeformed configuration.
By default, linearly applies pressure from `t = 0` to `t = 1`
 `1`
*  `model`
 Material model to use (`elasticitylinear`, `elasticityneohookeancurrent`, `elasticitymooneyrivlininitial`, etc.)
 `elasticitylinear`
*  `forcing`
 Forcing term option (`none`, `body`, or `mms`)

*  `forcing_body_vector [ax,ay,az][,a2x,a2y,a2z,...]`
 Userspecified acceleration vectors for applying body forces. Scaled by the mass computed with material density `{material name}_rho` and nodal volume. If more than one vector is specified, transition times must be provided as `forcing_body_times [t1,t2,...]`.

*  `forcing_body_times [t1,t2,...]`
 Transition times between each acceleration vector.
Note: If the first specified time is after `0`, an acceleration vector of `0,0,0` will be added with time `0` in order to ramp body forces.
By default, linearly applies acceleration from `t = 0` to `t = 1`

*  `forcing_body_interpolation`
 Interpolation type between specified acceleration vectors (`none` or `linear`).

*  `ceed_field_[fieldnumber]_mat_type [MatType]`
 Submatrix `MatType` for a `MATCEED` submatrix for a single solution field
 `MATCEED`
*  `ceed_[fieldname]_mat_type [MatType]`
 Submatrix `MatType` for a `MATCEED` submatrix for a single solution field
 `MATCEED`
*  `pc_type`
 PC type for linear solver
 `pmg` (most problems), `gamg` (linear problems with single active field), or `jacobi` (problems with multiple active fields)
*  `pmg_coarsening_type`
 PMultigrid coarsening to use (`logarithmic`, `uniform`, or `user`)
 `logarithmic`
*  `pmg_level_orders [int list]`
 Array of orders for each multigrid level, in ascending order; fine grid order specified by `orders`.
This is only used with `pmg_coarsening_type` `user`.

*  `pmg_coarse_order [int]`
 Polynomial order of coarse grid basis functions for materials with one field.
This is only used with `pmg_coarsening_type` of `logarithmic` or `uniform`.
 `1`
*  `surface_force_faces [int or string list]`
 List of named faces or face set label values on which to compute surface force and centroids.

*  `surface_force_face_[facename]_label_value [int]`
 Face set label value for a given `facename`. Optional only if `facename` is an integer corresponding to a face set label value.

*  `surface_force_face_[facename]_bounding_box [xmin ymin zmin xmax ymax zmax]`
 Optional bounding box specifying a subregion of a face set label value on which to compute surface forces and centroids. Useful for meshes which lack labeled faces.

*  `q_extra_surface_force [int]`
 Increased quadrature space order for celltoface surface force computation; final order given by `order[0] + q_extra_surface_force`
 `1`
*  `expected_strain_energy [real]`
 Expected strain energy, for testing

*  `expected_max_displacement_[direction] [displacement]`
 Expected max displacement in a particular direction (`x`, `y`, or `z`), for testing

*  `expected_surface_force_face_[facenumber]_[direction] [force]`
 Expected surface force on face `facenumber` in a particular direction (`x`, `y`, or `z`), for testing

*  `expected_surface_force_face_[facenumber] [fx,fy,fz]`
 Expected surface forces on face `facenumber`, overrides any `expected_surface_force_face_[facenumber]_[direction]`, for testing

*  `expected_centroid_face_[facenumber]_[direction] [value]`
 Expected centroid of face `facenumber` in a particular direction (`x`, `y`, or `z`), for testing

*  `expected_centroid_face_[facenumber] [cx,cy,cz]`
 Expected centroid of face `facenumber`, overrides any `expected_centroid_face_[facenumber]`, for testing

*  `view_diagnostic_quantities viewer:filename.extension`
 Output final solution for viewing, ASCII format to STDOUT is used if no viewer is passed

*  `view_swarm ascii:[base_filename].xmf`
 Output final MPM fields at material points for viewing, only `XDMF` format is currently supported. Only supported for `method mpm`.

*  `ts_monitor_strain_energy`
 Output computed strain energy on each time step

*  `ts_monitor_diagnostic_quantities viewer:filename.extension`
 Output final solution for viewing, ASCII format to STDOUT is used if no viewer is passed

*  `skip_diagnostic_quantities`
 Skip diagnostic quantities computation all together after the simulation completes.

*  `ts_monitor_surface_force [ascii:filename.csv]`
 Output centroid displacements and accurate surface forces computed using the volumetric residual operator (reaction force) for faces given by `surface_force_faces` on each time step.
Only CSV or plain text output is supported.
If no filename is provided, results are printed to the terminal (`stdout`).

*  `ts_monitor_surface_force_per_face [ascii:base_filename.csv]`
 Like `ts_monitor_surface_force`, except that a separate file is created for each face provided to `surface_force_faces`.
The created files are named `[base filename]_[face name].csv`.

*  `ts_monitor_surface_force_cell_to_face`
 Output centroid displacements and approximate surface forces computed using celltoface quadrature for faces given by `surface_force_faces` on each time step.
This option is extremely inaccurate depending on the boundary conditions and geometry.
Generally, you should use `ts_monitor_surface_force` instead.

*  `ts_monitor_swarm ascii:[base_filename].xmf`
 Monitor swarm fields at each timestep, saving an XDMF file `[base_filename].xmf` which can be read by Paraview and
one binary file `[base_filename]_k.pbin` per timestep `k` which are automatically referenced and indexed by the XDMF file.
Only supported for `method mpm`.

*  `ts_monitor_checkpoint [filename]`
 Output binary file with solution checkpoints for continuation.
Note: Binary viewer and extension are always used.

*  `ts_monitor_checkpoint_toggle`
 Toggle between writing two checkpoint files, `filename0.bin` and `filename1.bin`.

*  `checkpoint_final_solution [filename]`
 Output binary file with final solution checkpoint.
Note: Automatic with `ts_monitor_checkpoint`.

*  `ts_monitor_*_interval [int]`
 Number of time steps between monitor output, for any of `ts_monitor_*` options above
 `1`
*  `ts_view`
 View PETSc `TS` time stepper configuration

*  `snes_view`
 View PETSc `SNES` nonlinear solver configuration

*  `log_view`
 View PETSc performance log

*  `ts_monitor_reaction_force`
 Deprecated: Use `ts_monitor_surface_force`

*  `help`
 View comprehensive information about runtime options

:::
To verify the convergence of the linear elasticity formulation on a given mesh with the method of manufactured solutions, run:
```console
$ ./bin/ratelquasistatic dm_plex_filename [mesh] order [order] model elasticitylinear 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.
:::{listtable} Material Property and Model Options
:headerrows: 1
*  Option
 Description
 Model
*  `E [real]`
 [Young's modulus](https://en.wikipedia.org/wiki/Young%27s_modulus), $E > 0$
 NeoHookean
*  `nu [real]`
 [Poisson's ratio](https://en.wikipedia.org/wiki/Poisson%27s_ratio), $\nu < 0.5$
 NeoHookean, MooneyRivlin or Ogden
*  `nu_smoother [real]`
 Poisson's ratio for multigrid smoothers, $\nu < 0.5$
 NeoHookean, MooneyRivlin or Ogden
*  `mu_1 [real]`
 [MooneyRivlin material constant](https://en.wikipedia.org/wiki/Mooney–Rivlin_solid), $\mu_1 > 0$,
 MooneyRivlin
*  `mu_2 [real]`
 [MooneyRivlin material constant](https://en.wikipedia.org/wiki/Mooney–Rivlin_solid), $\mu_2 > 0$
 MooneyRivlin
*  `m [m_1, m_2, m_3]`
 [Ogden material constant](https://en.wikipedia.org/wiki/Ogden_hyperelastic_model)
 Ogden
*  `alpha [alpha_1, alpha_2, alpha_3]`
 [Ogden material constant](https://en.wikipedia.org/wiki/Ogden_hyperelastic_model), $2 \secondlame = \sum_{j=1}^N m_j \alpha_j,$ with $m_j \alpha_j > 0$
 Ogden
*  `yield_stress [real]`
 [Initial yield stress threshold](https://en.wikipedia.org/wiki/Plasticity_(physics)), $\sigma_0 > 0$
 Linear Plasticity
*  `hardening_A [real]`
 [Isotropic hardening parameter](https://en.wikipedia.org/wiki/Plasticity_(physics)), $A > 0$
 Linear Plasticity
*  `use_AT1 [bool]`
 True (default): AT1 model, False: AT2
 Phase Field Modeling of Fracture
*  `use_offdiagonal [bool]`
 True (default): full Jacobian, False: Jacobian diagonal terms only (for quasiNewton methods),
 Phase Field Modeling of Fracture
*  `fracture_toughness [real]`
 [Fracture_toughness expressed as critical energy release rate](https://en.wikipedia.org/wiki/Energy_release_rate_(fracture_mechanics)), $fracture_{toughness} > 0$
 Phase Field Modeling of Fracture
*  `characteristic_length [real]`
 Length scale parameter of phasefield model, $characteristic_{length} > 0$
 Phase Field Modeling of Fracture
*  `residual_stiffness [real]`
 Residual stiffness in full fracture state ($\phi = 1$), $residual_{stiffness} > 0$
 Phase Field Modeling of Fracture
*  `damage_viscosity [real]`
 Viscosity for viscous regularization of damage problem, $damage_{viscosity} >= 0$
 Phase Field Modeling of Fracture
:::
(multiplematerials)=
## 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 {code}`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 {code}`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 {code}`{material name}_`) to specify other aspects for each material at runtime.
We also specify, for each material, which domain label values to use with {code}`rod_label_value 3 binder_label_value 4`.
To define material parameters such as $E$ and $\nu$, we now use {code}`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:
```console
$ ./bin/ratelquasistatic material rod,binder rod_model elasticitymooneyrivlininitial rod_mu_1 0.5 rod_mu_2 0.5 rod_nu 0.4 binder_label_value 3 binder_model elasticityneohookeaninitial 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:
:::{listtable} Multiple Material Runtime Options
:headerrows: 1
*  Option
 Description
 Default value
*  `material [string list]`
 List of names to use as labels for each material.

*  `{material name}_model`
 Material to use (`elasticitylinear`, `elasticityneohookeancurrent`, `elasticitymooneyrivlininitial`, etc.) for a given material.
 `elasticitylinear`
*  `{material name}_label_name`
 Domain label specifying the type of volume to use for specifying materials.
Optional.
 `"Cell Sets"`
*  `{material name}_label_value [int]`
 Domain value specifying the volume to use for a given material.

*  `{material name}_rho [real]`
 Density of materal, by default in kg/m^3
 `1`
*  `{material name}_E [real]`
 [Young's modulus](https://en.wikipedia.org/wiki/Young%27s_modulus), $E > 0$

*  `{material name}_nu [real]`
 [Poisson's ratio](https://en.wikipedia.org/wiki/Poisson%27s_ratio), $\nu < 0.5$

*  `{material name}_nu_smoother [real]`
 Poisson's ratio for multigrid smoothers, $\nu < 0.5$

*  `{material name}_forcing`
 Forcing term option (`none`, `body`, or `mms`).
Overrides global forcing option provided with `forcing`.
 `none`
*  `{material name}_forcing_body_vector [ax,ay,az][,a2x,a2y,a2z,...]`
 Userspecified acceleration vectors for applying body forces.
Scaled by the mass computed with material density `{material name}_rho` and nodal volume.
If more than one vector is specified, transition times must be provided as `forcing_body_times [t1,t2,...]`.
Overrides global forcing option provided with `forcing_body_vector`.
 `0,0,0`
*  `{material name}_forcing_body_times [t1,t2,...]`
 Transition times between each acceleration vector.
Note: If the first specified time is after `0`, an acceleration vector of `0,0,0` will be added with time `0` in order to ramp body forces.
By default, linearly applies acceleration from `t = 0` to `t = 1`.
Overrides global forcing option provided with `forcing_body_times`.
 `1`
*  `{material name}_forcing_body_interpolation`
 Interpolation type between specified acceleration vectors (`none` or `linear`).
Overrides global forcing option provided with `forcing_body_interpolation`.
 `linear`
:::
An example of specifying a two material quasistatic solve with YAML is provided in {code}`examples/ex02quasistaticelasticitymultimaterial.yml`.
## Algebraic Solvers
The examples are configured to use the following NewtonKrylovMultigrid method by default.
 Newtontype 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 {code}`mg_levels_ksp_max_it 2`, for example.)
Application of the linear operators for all levels with order $p > 1$ is performed matrixfree 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 commandline 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 commandline 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.
:::{listtable} (Non)dimensionalization options
:headerrows: 1
*  Option
 Description
 Default value
*  `units_meter`
 1 meter in scaled length units
 `1`
*  `units_second`
 1 second in scaled time units
 `1`
*  `units_kilogram`
 1 kilogram in scaled mass units
 `1`
:::
For example, consider a problem involving metals subject to gravity.
:::{listtable} Characteristic units for metals
:headerrows: 1
*  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., {code}`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, {code}`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, $\trace \bm{E}$, $\trace \bm{E}^2$, $ J $, and strain energy density $\psi$.
The table below summarizes the formulations of each of these quantities for each material type.
:::{listtable} Diagnostic quantities
:headerrows: 1
*  Quantity
 Linear elasticity
 NeoHookean hyperelasticity
*  Cauchy stress tensor
 $\bm{\sigma}$
 $\bm{\sigma} = \bm{F} \bm{S} \bm{F}^T / J $
*  Hydrostatic pressure
 $\trace \bm{\sigma} / 3$
 $\trace \bm{\sigma} / 3$
*  Volumetric strain
 $\trace \bm{\varepsilon}$
 $\trace \bm{E}$
*  $\trace \bm{E}^2$
 $\trace \bm{\varepsilon}^2$
 $\trace \bm{E}^2$
*  $ J $
 $1 + \trace \bm{\varepsilon}$
 $ J $
*  Strain energy density
 $\frac{\lambda}{2} (\trace \bm{\varepsilon})^2 + \mu \bm{\varepsilon} : \bm{\varepsilon}$
 $\frac{\lambda}{4}\left(J^2  1  2 \log J \right) + \mu \trace \bm{E}  \mu \log J$
*  von Mises stress
 $\sqrt{\frac 3 2 \bm{\hat \sigma} \tcolon \bm{\hat \sigma}}$
 $\sqrt{\frac 3 2 \bm{\hat \sigma} \tcolon \bm{\hat \sigma}}$
*  Mass Density
 $\rho_0 / J$
 $\rho_0 / J$
:::
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.
Alternatively, one can skip all diagnostic evaluations with `skip_diagnostic_quantities` if no diagnostic quantities are needed after the simulation finishes running.
[cubit]: https://cubit.sandia.gov/
[this repository]: https://github.com/jeremylt/ceedSampleMeshes
## Boundary Conditions
### Contact
Ratel supports frictionless and frictional contact with a levelset plane via the `bc_platen` command line option.
See [Platen Contact Boundary Conditions](modeling/governingequations/contactplaten) for details on the theory of Ratel's contact enforcement methods and
see [Friction Models](modeling/governingequations/friction) for details on the different friction models available in Ratel.
The [Contact Options Table](table_contact_options) explains the commandline options available for contact boundary conditions.
For brevity, the string `[prefix]` is used in place of the full prefix `bc_platen_[platen_name]` in the option listings.
(table_contact_options)=
:::{listtable} Contact Options
:headerrows: 1
:widths: 40 50 10
*  Option
 Description
 Default Value
*  `bc_platen [string list]`
 List of labels or names for each platen (halfplane) contact boundary condition to apply. Examples: "top,bottom" or "1,2".
If integer values are provided, then they are assumed to correspond to surface attribute tags in the mesh.
Otherwise, `[prefix]_label_value [int]` must be set for each face with a noninteger name.

*  `[prefix]_type [nitschepenalty]`
 Solver method to use for platen boundary, either `nitsche` for Nitsche's method or `penalty` for penalty method.
 `nitsche`
*  `[prefix]_label_value`
 Value of `DMPlex` label to apply the platen to (such as the face label). If `[platen_name]` is a string then the label value must be provided.
 `[platen_name]` if `[platen_name]` is an integer.
*  `[prefix]_center [cx,cy,cz]`
 Specify the center of the platen, with components given with respect to the global coordinate system

*  `[prefix]_normal [nx,ny,nz]`
 Specify the exterior normal to the platen, with components given with respect to the global coordinate system.
This vector should point toward the face `[facenumber]`.

*  `[prefix]_distance [dist][,dist2,dist3,...]`
 Distance(s) of the halfplane along the specified normal vector.
In the context of timestepping, the speed of the platen depends on the value of `[prefix]_interpolation`.
If more than one distance is specified, transition times must be provided as `[prefix]_times [t1,t2,...]`.
 `0.0`
*  `[prefix]_times [t1,t2,...]`
 Transition times between each platen distance value, primarily used to control the platen velocity.
Note: If the first specified time is after `0`, a distance of `0` will be added implicitly with time `0` in order to start from an undeformed configuration.
Note: If a single distance is provided, the time value defaults to `1`; i.e., the platen will move the prescribed distance in `1` time unit.
 `1`
*  `[prefix]_interpolation`
 Interpolation type between specified distance values (`none` or `linear`).
Note: `none` results in piecewise constant displacement while `linear` results in piecewise linear displacement and piecewise constant velocity.
 `linear`
*  `[prefix]_gamma [real]`
 Nitsche's method penalty parameter, larger values result in less erroneous penetration. Generally, should be ~100 times the Young's modulus.
 `1.0`
*  `[prefix]_friction_type [nonecoulombthrelfall]`
 Specify the type of friction to use, see [Friction Models](modeling/governingequations/friction) for details on available models.
 `none`
*  `[prefix]_friction_kinetic [nonnegative real]`
 Kinetic (sliding) coefficient of friction $\mu_k$, unitless.
 `0.1`
*  `[prefix]_friction_static [nonnegative real]`
 Static (slipping) coefficient of friction $\mu_s > \mu_k$, unitless. Not currently used.
 `0.15`
*  `[prefix]_friction_viscous [nonnegative real]`
 Viscous damping coefficient $F_v$, units of $\frac{\mathrm{N}\cdot\mathrm{s}}{\mathrm{m}}$.
 `0.0`
*  `[prefix]_friction_tolerance_velocity [positive real]`
 Tolerance velocity $v_0$ at which full frictional slipping is permitted, units of $\frac{\mathrm{m}}{\mathrm{s}^2}$. Only used by Threlfall friction model.
 `0.05`
:::
:::{note}
It is often easier to specify commandline arguments in YAML format, since repeated prefixes can be replaced with a YAML dictionary.
For example, consider the following commandline arguments specifying a platen boundary condition named `top` with friction on face with attribute label value `1`:
```
bc_platen top bc_platen_top_label_value 1 bc_platen_top_normal 1,0,0 bc_platen_top_center 0,0,0 bc_platen_top_distance 0.1 bc_platen_top_gamma 500 bc_platen_top_friction_type coulomb bc_platen_top_friction_kinetic 0.4 bc_platen_top_friction_viscous 0.01
```
Alternatively, the same options specified via a YAML options file are far more readable:
```yaml
# platen_options.yml
bc:
platen: top
platen_top:
label:
value: 1
normal: 1,0,0
center: 0,0,0
distance: 0.1
gamma: 500
friction:
type: coulomb
kinetic: 0.4
viscous: 0.01
```
The options can then be passed to Ratel via the `options_file platen_options.yml` command.
:::