Running a forward problem
Once the CALIBR8 project has been compiled and the environment has been loaded with the command capp load (see the instructions Compiliation.), running a forward problem is as simple as calling the CALIBR8 executable primal, which should now exist in your PATH with an input YAML file.
primal <input.yaml>
Example Input YAML FILE
Below are the contents of an example input YAML file, that we will go through line by line in subsequent sections:
example_input:
problem:
name: J2_finite_2D
discretization:
geom file: 'notch2D.dmg'
mesh file: 'notch2D.smb'
assoc file: 'notch2D.txt'
num steps: 8
step size: 1.
residuals:
global residual:
type: 'mechanics'
nonlinear max iters: 15
nonlinear absolute tol: 1.e-12
nonlinear relative tol: 1.e-12
print convergence: true
local residual:
type: 'hyper_J2_plane_strain'
nonlinear max iters: 500
nonlinear absolute tol: 1.e-12
nonlinear relative tol: 1.e-12
materials:
body:
E: 1000.
nu: 0.25
K: 100.
Y: 10.
Y_inf: 0.
delta: 0.
# bc name: [resid_idx, eq, node_set_name, value]
dirichlet bcs:
expression:
bc 1: [0, 0, xmin, 0.0]
bc 2: [0, 1, ymin, 0.0]
bc 3: [0, 1, ymax, 0.001 * t]
linear algebra:
Linear Solver Type: "Belos"
Preconditioner Type: "Teko"
Linear Solver Types:
Belos:
Solver Type: "Block GMRES"
Solver Types:
Block GMRES:
Convergence Tolerance: 1.e-12
Output Frequency: 10
Output Style: 1
Verbosity: 33
Maximum Iterations: 200
Block Size: 1
Num Blocks: 200
Flexibile Gmres: false
VerboseObject:
Output File: "none"
Verbosity Level: "none"
Preconditioner Types:
Teko:
Inverse Type: "BGS2x2"
Write Block Operator: false
Test Block Operator: false
Inverse Factory Library:
BGS2x2:
Type: "Block Gauss-Seidel"
Use Upper Triangle: false
Inverse Type 1: "AMG2"
Inverse Type 2: "AMG1"
AMG2:
Type: "MueLu"
number of equations: 2
verbosity: "none"
'problem: symmetric': false
AMG1:
Type: "MueLu"
verbosity: "none"
number of equations: 1
'problem: symmetric': false
GS:
Type: "Ifpack2"
Overlap: 1
Ifpack2 Settings:
'relaxation: type': "Gauss-Seidel"
Problem
The problem block will specify various aspects of the problem that you are about to run. In this case, we are only specifying a variable called name, which will uniquely name the primal run. All output from this run will be output to the directory name.
problem:
name: J2_finite_2D
Discretization
The discretization block will specify all aspects of an individual problem’s discretization. For all problems, we require a geometric model, a mesh of that geometric model, and an associations file linking together collections of geometric objects to a unique string. The generation and usage of these files is nontrivial and is covered in depth in a different section (TODO PUT A REFERENCE HERE ONCE THIS IS DOCUMENTED).
The number of steps and the step size determines how the problem is loaded. In this example, we take 8 load steps with a psuedo-time increment of \(\Delta t = 1.0\). Later on, in the boundary conditions block, this pseudo-time \(t\) will be used to specify boundary conditions at load increments. (THIS SYNTAX MAY CHANGE AS WE MOVE TO CONSIDER TRUE TRANSIENT PHYSICS AND NOT QUASI-STATIC BEHAVIOR).
Additionally, there are some pre-included geometries and meshes for use in testing CALIBR8 available in the repository.
discretization:
geom file: 'notch2D.dmg'
mesh file: 'notch2D.smb'
assoc file: 'notch2D.txt'
num steps: 8
step size: 1.
Residuals
In general, CALIBR8 considers the coupling of two residual systems: a global residual and a local residual. In this case, the global residual corresponds to the overall governing kinematic equations (the balance of linear momentum in the absence of inertial terms) and the local residual corresponds to the constitutive model equations solved at each integration point inside of an element. Here, we have specified some parameters that are largely self explanatory.
Of note, perhaps, is that we have chosen a 2D plane strain finite deformation plasticity model. For this model, we have chosen some benign material parameters for the elastic modulus \(E\), Poisson’s ratio \(\nu\), the yield strength \(Y\), the linear hardening modulus \(K\), and have set other parameters to \(0\).
residuals:
global residual:
type: 'mechanics'
nonlinear max iters: 15
nonlinear absolute tol: 1.e-12
nonlinear relative tol: 1.e-12
print convergence: true
local residual:
type: 'hyper_J2_plane_strain'
nonlinear max iters: 500
nonlinear absolute tol: 1.e-12
nonlinear relative tol: 1.e-12
materials:
body:
E: 1000.
nu: 0.25
K: 100.
Y: 10.
Y_inf: 0.
delta: 0.
Boundary Conditions
In the dirichlet bcs block, we set up some simple boundary conditions to constrain rigid body rotations/translations, and pull our geometry at an increment of \(0.01*t\) on the top y face of the notch specimen domain.
Note that, as the comment suggests, the DBC input structure has the form: [residual index, equation index, node set name, value as a string]. The node set name comes from the associations file assoc.txt set in the discretization block, and the value is a run-time-compiled string expression that can be fairly sophisticated.
# bc name: [resid_idx, eq, node_set_name, value]
dirichlet bcs:
expression:
bc 1: [0, 0, xmin, 0.0]
bc 2: [0, 1, ymin, 0.0]
bc 3: [0, 1, ymax, 0.001 * t]
Linear Algebra
The linear algebra block should remain largely untouched unless you are an experienced user. Of particular note, however, is that the block below should change from 2 to 3 when switching from a 2D to a 3D problem.
AMG2:
Type: "MueLu"
number of equations: 2
verbosity: "none"
'problem: symmetric': false