[KeganLeckness]

Hi all,

I'm modeling high intensity pressure propagation through the ear. Pressure is applied at the ear canal entrance and a two-way FSI is defined at the other end of the canal at the eardrum. I've had a tremendous amount of difficulty with diverging solutions, "Cannot read Total Mesh Displacement at FSI," and "Negative element volume" errors. I believe my issues (stemming from large eardrum displacements) would be resolved by re-meshing the fluid domain when the mesh becomes poor.

EDR has two good re-meshing tutorials. I cannot use the ICEM CFD method, as it is only applicable in the case of purely translational mesh displacement. The Workbench re-meshing method [in the example the part is a rotating fan] requires a geometric parameter to be updated in the batch (running in background) Workbench project. In this example, the mesh and part motion are known and set by the user.

I am unable to use this approach, as the degree of mesh deformation is unknown -- I have no geometric parameter.

My plan is as follows:

• Initialize Interruption Control that pauses the simulation after some threshold of mesh deformation
• Output geometry file at current timestep (with deformations)
• Implement (after devising) journal code that opens up a batch Workbench project with only Geometry and Mesh cells. Workbench script reads output geometry file and meshes it. [This action is initiated by a Configuration]
• New mesh is sent back to CFX analysis, simulation resumes. Repeat if necessary

Those of you with re-meshing experience, does this seem reasonable?
How can I output the current-timestep geometry file such that it may be read by the batch Workbench project script?


The two tutorials are below:
http://www.edr.no/en/courses/ansys_icem_cfd
http://www.edr.no/blogg/ansys_blogge...nch_cfx_remesh


Thank you

[mvoss]

Can you post a schematic on how the domain looks like and give an estimation about the expected displacement?
"Reading displacment error"-->ANSYS Problem,
"negative volume error"-->large displacement in one timestep and maybe poor mesh displ. convergence

[KeganLeckness]

The geometry can be seen in Mesh.jpg. The length of the canal is 30 mm. Impulse pressure (duration: 0 to 3 ms) is applied at a small circle on the showing face of the rectangular domain. The FSI is at the end of the cylinder.

These are results from an analysis terminated through Interruption Control precisely at the timestep I received a Negative Element Volume error. I monitored the Minimum Orthogonality Angle for both domains, as pictured, and we can see it go negative, indicating negative element volume. I also monitored the Mesh Displacement, Mesh Velocity, and Aspect ratio of both domains. The mesh displacement and mesh velocity spike towards the end of the simulation, with the canal domain's values being two orders higher than in the box domain. Similarly, the aspect ratio of the canal domain spikes while the box domain's stays the same. The location of the negative element volume, however, is shown to be in the box. How could this be, when all measures of poor mesh quality are shown to be in the canal domain?

The total mesh displacement during the last timestep is on the order of microns.

Thank you for your response
Kegan

[mvoss]

Please check for the pictures...

[KeganLeckness]

That's embarrassing. Let's see if this works.

[singer1812]

This is FSI with ANSYS FEA?

Unless they have altered features in the latest revision, CFX/ANSYS can't handle FSI with remesh without very advanced techniques and scripting on APDL side (ANSYS doesnt support this).

Fluent will allow a remesh with FSI.

[mvoss]

I have no idea about why the error rises up in the rect-domain. There should be basically be no problem with neg. element if the displacement is of order µm and the elementsize is reasonably bigger.
You should run a case with GIVEN displacement where and how big you expect it to be in the FSI-run - this is how and what i always check before starting a time consuming FSI-run.
Simply disable the calculation for the fluid, temp, whatever in the expert-section, calculate the displacement solely and write out the mesh every timestep. Hope you get the idea.
AND: i would highly recommend using a nice hex-mesh, which is pretty easy for this geom. !

[KeganLeckness]

Thank you for the advice!

Update:

It appears this remeshing scheme is difficult, as Singer mentioned.

I have successfully implemented a workbench script in conjuncture with an ICEM script that (when ran on a new WBPJ) opens batch ICEM, pulls final deformed mesh from a CFX analysis (.res rile), turns the mesh into geometry for remeshing, writes new .cfx5, and exits ICEM.

The problem, however, is that this only allows for remeshing when the CFX/ANSYS analysis is complete. To issue a remeshing command in CFX (for mid-simulation remeshing), you must use a Configuration. Configurations cannot be implemented in FSI cases, however. The error ".. configuration not physically valid" appears during coupled analyses.

I think small changes in my code would have allowed me to remesh as planned, were configurations able to be used in coupled simulations.

I have since moved on to Fluent.

I will post the remeshing code I tried.

Workbench script:

# encoding: utf-8
SetScriptVersion(Version="15.0")

import os

from System.Diagnostics import Process
p = Process()
p.StartInfo.UseShellExecute = False
p.StartInfo.RedirectStandardOutput = False

p.StartInfo.FileName = 'C:\\Program Files\\ANSYS Inc\\v150\\icemcfd\\win64_amd\\bin\\icemcfd.bat'

p.StartInfo.Arguments = '<path to ICEM .rpl script>'

p.Start()
p.WaitForExit()
exit

This opens batch ICEM, runs the .rpl script, closes ICEM.

ICEM .rpl script

ic_empty_tetin
ic_run_application_exec . icemcfd/output-interfaces cfx2df {-s0 {C:/Users/leck7795/Desktop/ReMeshing/ICEM_final res_files/dp0/CFX/CFX/Fluid Flow CFX_001.res} {C:/Users/leck7795/Desktop/ReMeshing/WORKING ICEM CFD_files/dp0/ICM/ICEMCFD/tmpdomain.uns}}
ic_uns_load {{C:/Users/leck7795/Desktop/ReMeshing/WORKING ICEM CFD_files/dp0/ICM/ICEMCFD/tmpdomain.uns}} 3 0 {}
ic_geo_new_family PART0
ic_uns_move_family_elements ORFN PART0
ic_boco_solver
ic_uns_update_family_type visible {WALL INLET ORFN FSI DEFAULT-DOMAIN PART0} {TRI_3 !TETRA_4} update 0
ic_boco_clear_icons
ic_csystem_display all 0
ic_csystem_set_current global
ic_boco_nastran_csystem reset
ic_uns_diag_reset_degen_min_max


ic_uns_build_mesh_topo All -angle 150 -smart
ic_geo_import_mesh {} 1 1 0
ic_geo_set_modified 1
ic_csystem_display all 0
ic_csystem_set_current global
ic_boco_nastran_csystem reset
ic_unload_mesh
ic_uns_diag_reset_degen_min_max
ic_delete_empty_parts


Remeshing scheme here (i.e. sizing, meshing methods)

ic_uns_check_duplicate_numbers
ic_uns_renumber_all_elements 1 1
ic_save_unstruct {<path to save .uns mesh>}
ic_uns_set_modified 1

ic_boco_solver
ic_boco_solver {ANSYS CFX}
ic_solution_set_solver {ANSYS CFX} 1
ic_boco_save {<.fbc path>}
ic_boco_save_atr {<atr path>}

ic_exec {C:/Program Files/ANSYS Inc/v150/icemcfd/win64_amd/icemcfd/output-interfaces/cfx5} -dom {C:/Users/leck7795/Desktop/ReMeshing/trash_scripts/ICM.uns} -b {C:/Users/leck7795/Desktop/ReMeshing/trash_scripts/ansys.fbc} -ascii -db -internal_faces {C:/Users/leck7795/Desktop/ReMeshing/trash_scripts/ICM.cfx5}

exit


imports mesh from .res
mesh -> geometry. deletes imported mesh
saves .uns mesh file. must be done before exportation to other formats is allowed
saves attribute files, new .cfx5 mesh, and exits ICEM