Creating structural models
The data and properties of each structural model are defined through a set of definitions in a .m script. These properties are stored in struct data structures. The following structs must be defined and provided as input to the ONSAS function in this order:
materialselementsboundaryCondsinitialCondsmeshnumericalMethodotherParams
Each struct has its own fields with specific names, used to store each corresponding property or information. Each field is obtained or assigned using structName.fieldName. A description of each struct and its fields follows at next.
The materials struct
The materials struct contains the information of the material behavior considered for each element.
material.hyperElasModel
This is a cell array with the string-names of the material models used, the options for these names are:
'linearElastic': for linear behavior in small strains and displacements. The scalar parameters of this model are $p_1=E$ the Young modulus and $p_2=\nu$ the Poisson's ratio.'SVK': for a Saint-Venant-Kirchhoff material where the parameters $p_1$ and $p_2$ are the Lamé parameters and $\textbf{E}$ is the Green-Lagrange strain tensor, with the strain-energy density function given by
\[\Psi( \textbf{E} ) = \frac{p_1}{2} tr(\textbf{E})^2 + p_2 tr(\textbf{E}^2) \quad p_1 = \frac{ E \nu }{ (1+\nu) (1-2\nu) } \quad p_2 = \frac{ E }{ 2 (1+\nu) }\]
'NHC': for a Neo-Hookean compressible material. The model implemented is given by
\[\Psi( \textbf{C} ) = \frac{p_1}{2} ( tr(\textbf{C})-3 -2 L( \sqrt{det(\textbf{C})} ) ) + \frac{p_2}{2} \left( \sqrt{det(\textbf{C})}-1 \right)^2 \quad p_1 = \frac{ E }{ 2 (1+\nu) } \quad p_2 = \frac{ E }{ 3 (1-2 \nu) }\]
'isotropicHardening': an ElastoPlastic material with isotropic hardening given by the von mises flow rule for the plane strain element. The parameters are introduced as: REVISAR!! $p_1=E$ , $p_2 = K$ and $p_3=\sigma_{Y,0}$.
materials.hyperElasParams
A cell structure with vectors with the material properties of each material used in the model. The $i$-th entry of the cell, contains a vector like this:
\[[ p_1 \dots p_{n_P} ]\]
where $n_P$ is the number of parameters of the constitutive model and $\mathbf{p}$ is the vector of constitutive parameters.
material.density
This is a cell with the scalar values of the densities of the materials used in the model.
material.nodalMass
This fields sets a vector of nodal masses components $[m_x, m_y, m_z]$ that is assigned to nodes.
The elements struct
The elements struct contains the information about the type of finite elements used and their corresponding parameters.
elements.elemType
A cell structure with the string-names of the elements used: node, truss, frame, triangle or tetrahedron. Other auxiliar types such as edge are also available
elements.elemTypeParams
A cell structure with auxiliar params information, required for some element types:
trianglevector with parameters, the first parameter is an integer indicating if plane stress (1) or plane strain (2) case is considered.
elements.massMatType
The massMatType field sets, for frame or truss elements, whether consistent or lumped mass matrix is used for the inertial term in dynamic analyses. The massMatType field should be set as a string variable: 'consistent' or 'lumped', and if it is not declared then by default the 'lumped' mass matrix is set.
elements.elemCrossSecParams
This is a cell structure with the information of the geometry of the element.
1D elements
For truss or frame elements, this cell has two entries, first a string with a name of the type of cross section, and in the second entry a vector of real parameters setting the shape of that section:
\[\{ crossSectionTypeString, \,\, [ crossSectionParam_{1}, \,\,\dots,\,\, crossSectionParam_{n} ] \}\]
with $n$ being the number of parameters of the cross section type, and crossSectionTypeString the type of cross section. The possible cross section strings and their corresponding properties are:
generic:general sections, where areas and inertias are provided as parameters according to the vector: $[A \,\, J \,\, I_{yy} \,\, I_{zz} \,\, I_{\rho}(1,1) \,\, I_{\rho}(2,2) \,\, I_{\rho}(3,3) ] $ where $A$ is the area, $I_{ii}$ is the second moment of inertia of the cross-section respect to $i$ direction, $J$ is the polar moment of inertia and $I_{\rho}$ is the inertia tensor.rectangle: rectangular sections where thicknesses $t_y$ and $t_z$ are provided as the vector $[t_y, t_z]$circle: circular sections where diameter is provided.pipe: circular hollow section where external and internal diameters are provided as first and second entries of the vector of elementCrossSecParams.
For edge elements the thickness is expected (for 2D load computations).
See the crossSectionProps.m function for more details.
2D elements
For 2D elements such as triangle in this field a float number representing the thickness of the element is set.
elements.aeroNumericalParams
A cell with the number of Gauss integration points numGauss, the boolean computeStiffnessAeroTangent for computing the aerodynamic stiffness matrix and geometricNonLinearAero to take into account geometric nonlinearities or (reconfiguration).
\[\{ numGauss \,\,stiffnessAeroTangent\, \,geometricNonLinearAero \}\]
where the default cell is {4, false, true}
elements.dragCoefFunction, elements.liftCoefFunction and elements.pitchCoefFunction
If a frame aerodynamic analysis is desired, the drag, lift and pitch moment should be defined in this field. Each function receives Reynolds and the incidence angle as inputs and returns the the respective coefficient. For some elemCrossSecParams like 'circle' internal built-in functions are set as default.If any of the coefficients is defined considered then an empty [] struct is considered, this set this coefficient to zero.
elements.chordVector
A vector with the three coordinates of the aerodynamic chord vector (the system of coordinates considered for this is the local reference system at the undeformed configuration)
The boundaryConds struct
boundaryConds.loadsCoordSys
cell containing the coordinates system for the loads applied in each BC, each entry should be a 'global' string or a 'local', or an empty array if no load is applied in that BC setting [].
boundaryConds.loadsTimeFact
cell with the inline function definitions of load factors of the loads applied of an empty array.
boundaryConds.loadsBaseVals
cell with the (row) vector of the components of the load case
\[[ f_x, \, m_x, \, f_y, \, m_y, \, f_z, \, m_z ]\]
where $f_i$ are the components of forces and $m_i$ are the moments. Both forces or moments are considered per unit of length in the case of truss/frame/edge elements, or per unit of area in the case of triangle.
boundaryConds.userLoadsFileName
string with the filename of the .m function file provided by the user that can be used to apply forces not given by time-varying loadFactors. This function file should be placed in the example folder and it must receive two arguments: t (the time) and UsCell (a cell with: {the current displacement, velocity and acceleration} ). The function should one forces vector with the size of all the degrees of freedom of the problem (in global coordinates).
boundaryConds.imposDispDofs
cell with vectors of the local degrees of freedom imposed (integers from 1 to 6)
boundaryConds.imposDispVals
cell with vectors of the values of displacements imposed.
boundaryConds.springDofs
vector with the local degrees of freedom of the node with springs (integers from 1 to 6)
boundaryConds.springVals
vector with the values of the springs stiffnesses.
The mesh struct
The mesh struct contains the finite element mesh information.
mesh.nodesCoords
matrix with the coordinates of all the nodes of the mesh. The $i$-th row contains the three coordinates of the node $i$: $[x_i , \, y_i ,\, z_i]$,
mesh.conecCell
cell array with the elements and node-connectivity information. The $\{i,1\}$ entry contains the vector with the MEB (Material, Element, boundaryConds) indexes and the nodes of the $i$-th element. The structure of the vector at each entry of the cell is:
\[ [ materialInd, \, elementInd, \, boundaryCondInd, \, node_1 \dots node_{n} ]\]
where the first three indexes are natural numbers and $n$ is the number of nodes required by the type of element. If no property is assigned the $0$ index can be used, for instance, nodes used to introduced loads should be defined with materialIndex = 0.
The initialConds struct
If initial conditions are homogeneous, then an empty struct should be defined using initialConds = struct() ;. Otherwise the fields that can be set are:
initialConds.U: a vector of the displacements at time 0.initialConds.Udot: a vector of the velocities at time 0.initialConds.Udotdot: a vector of the accelerations at time 0.
The analysisSettings struct
This struct contains the parameters required to apply the numerical method for the resolution of the nonlinear equations:
methodName: string with the name of the method used:'newtonRaphson','arcLength','newmark','alphaHHT'.stopTolDeltau: float with tolerance for convergence in relative norm of displacements incrementstopTolForces: float with tolerance for convergence in relative norm of residual loadsstopTolIts: integer with maximum number of iterations per time stepdeltaT: time stepfinalTime: final time of simulationincremArcLen: with of cylinder for arcLength methoddeltaNM: delta parameter of newmark method. If this parameter is not declared then the classic Trapezoidal Newmark delta = $1/2$ is set.alphaNM: alpha parameter of newmark method. If this parameter is not declared then the classic Trapezoidal Newmark alpha = $1/4$ is set.alphaHHT: alpha parameter of alpha-HHT method. If this parameter is not declared then alpha=$-0.05$ is set.posVariableLoadBC: (parameter used by the arcLength method) this parameter is an integer with the entry of the boundaryConds cell corresponding with the loads vector affected by the load factoriniDeltaLamb: (parameter used by the arcLength method) this parameter sets the initial increment for the load factor $\lambda$.
another additional optional parameters are:
booleanSelfWeight: a boolean indicating if self weight loads are considered or not. The loads are computed using the density of the material and in the $-z$ global direction.iniMatUs: a matrix with initial solutions for each time step.
then the aerodynamic-frame element parameters set are
fluidProps: is a row cell with the density $\rho_f$, viscosity $\nu_f$ and the function with the fluid velocity
\[\{ \rho_f; \,\, \nu_f; \,\, 'fluidVelocity'\}\]
The otherParams struct
problemName: string with the name of the problem, to be used in outputs.plots_format: string indicating the format of the output. Use'vtk'for vtk output. default: no output.plots_deltaTs_separation: integer number N such that the time between vtk plots is N x deltaT.controlDofs: matrix with information of the degrees of freedom to compute and control. Each row should contain this form:[ node localdof ].storeBoolean: boolean to store the results of the current iteration such as the displacements, tangent matrices, normal forces and stresses. [default: 1]nodalDispDamping: scalar value of a linear viscous damping factor applied for all the displacement degrees of freedom [default: 0]