 |
v0.14.0 |
|
v0.14.0 |
Contact interaction between elastic solids having non-matching meshes in the contact interface.
Assumptions: small rotations, small strains, small relative tangential displacements (moderate if -convect option is switched on, see Contact parameters for more details).
Pairs of surfaces belonging to two solids that can potentially come into contact have to be marked as BLOCKSET_s, with one surface belonging to the pair with name MORTAR_MASTER and the other surface of the pair named MORTAR_SLAVE. An arbitrary number of pairs of contact surfaces can be defined by adding each side either in MORTAR_MASTER or in MORTAR_SLAVE _BLOCKSET.
NOTE: Springs can be used to eliminate the rigid body motion in a contact simulation under the pressure control.
Check the essential contact parameters in the file param_file.petsc:
NOTE: cn is the contact augmentation parameter which affects the convergence and has minimal effect on the solution (in a reasonable range of values). Recommended initial value is the Young's modulus of contacting solids (or harmonic mean in case of different values). The optimal value can be found by repetitively increasing/decreasing the initial value by e.g. a factor of 10.
| Name | Description | Default value |
|---|---|---|
-order | Approximation order of the field of spatial positions for the entire mesh | 1 |
-order_lambda | Approximation order of the field of contact Lagrange multipliers | 1 |
order_contact | Approximation order of the field of spatial positions for the contact elements and a given number of tetrahedral element layers adjacent to the contact interface | 1 |
-ho_levels_num | Number of tetrahedral element layers adjacent to the contact interface with higher order of the field of spatial positions (if -order_contact is higher than order) | 1 |
-cn_value | Augmentation parameter which affects the convergence and has minimal effect on the solution. Recommended initial value is the Young's modulus of contacting solids (or harmonic mean in case of different values). The optimal value can be found by repetitively increasing/decreasing the initial value by e.g. a factor of 10 | 1 |
-r_value | Contact regularisation parameter which can lie between 1.0 and 1.1. Values greater than 1 can speed-up the convergence, but will also alter the stiffness of the contact interface, therefore it is not recommended to change this parameter | 1 |
-step_num | Number of steps used to achieve the specified load value (so-called load control). Note that multi-stepping can be particularly important to obtain a solution for highly nonlinear problems | 1 |
-alm_flag | Defines the choice of the algorithm: 0 (False) - Complementarity function approach, 1 (True) - Augmented Lagrangian method | 0 |
-convect | If set to 1 (True), moderate relative tangential displacements can be taken into account | 0 |
First, the output h5m files need to be converted to vtk format. Note that these files can be converted one by one using the mbconvert tool:
or all at once by using the multiprocessing script convert.py:
The obtained vtk files can be viewed in Paraview, in particular:
out.vtk contains the stress tensor components (tag SPATIAL_POSITION_PIOLA1_STRESS), as well as material coordinates (tag MESH_NODE_POSITIONS) and current coordinates (tag SPATIAL_POSITION), which can be used to compute the displacement field with the Calculator filter as DISPLACEMENT=SPATIAL_POSITION-MESH_NODE_POSITIONSout_contact.vtk contains the nodal interpolation of the Lagrange multipliers equivalent to the contact pressure (tag LAGMULT)out_mortar_contact_integ_pts.vtk contains values of Lagrange multipliers (tag LAGMULT) and the normal gap (tag GAP) at Gauss points of the contact interface. Note that the Point Gaussian representation or alternatively the Glyph filter should be used for their visualisation in Paraview.Simulation taking into account non-matching-meshes contact and internal stress is possible using executable mortar_contact_thermal. Furthermore, this program provides possibility to save the value of the internal stress and the corresponding actual stress on the input mesh for subsequent use in the fracture module.
Two options are available for the internal stress:
thermal_strain in file mortar_contact_thermal.cppTwo options are available for saving the internal and corresponding actual stress on the mesh:
MED_INTERNAL_STRESS and MED_ACTUAL_STRESS, respectivelyINTERNAL_STRESS and ACTUAL_STRESS, respectivelyIn addition to outlined above parameters, the following parameters can be used with mortar_contact_thermal:
| Name | Description | Default value |
|---|---|---|
-analytical_input | If set to 1 (True), compute internal stress using analytical formula for thermal strain, otherwise use pre-computed internal stress saved on tags of the input mesh | 1 |
-thermal_expansion_coef | Value of thermal expansion coefficient for computing thermal strain (used if -analytical_input is set to 1) | 1e-5 |
-init_temp | Value of initial temperature for computing thermal strain (used if -analytical_input is set to 1) | 250.0 |
-stress_tag_name | Tag name used when reading internal stress from the mesh (if -analytical_input is set to 0) | INTERNAL_STRESS |
-save_mean_stress | If set to 1 (True), save mean values of internal and actual stress on the tags of the mesh, otherwise save integration point values of stresses | 1 |
-scale_factor | Scale for the internal stress | 1.0 |
-ignore_contact | If set to 1 (True), ignore contact | 0 |
-ignore_pressure | If set to 1 (True), ignore pressure | 0 |
-output_mesh_file | Name of the file for writing the mesh with internal and actual stress saved on tags | 0 |
Example of running the simulation using the analytical thermal strain for the internal stress and saving the mean values of the internal and external stress on the mesh:
