Learning Forum

[Jamasp]

I’m doing a simulation of a flow inside a channel using a FSI analysis by coupling transient structural and Fluent. This analysis has two phases. In the first phase, the structure significantly deforms and causes the tube (fluid domain) deforms as well. In the second phase, the structural deformation is minor but the fluid flows through the tube and it’s important to have a good quality of mesh to capture flow behavior.

What I want to do is to solve the first phase. Then generate a new mesh for the fluid domain using the deformed model from the last step in the first phase and start the second phase. Is it possible to do this in Fluent? I also used remeshing but not very useful. Remeshing does not give me a good quality of the mesh.

Please see the following example, which shows the last step from phase 1. I want to remesh the fluid domain (or possibly remesh the solid domain as well) before starting the second phase. The tube is squeezed and the mesh in the fluid domain highly changed and causes a very poor quality of mesh in the middle. As you can see, I used remeshing but not very helpful. I want the narrowed region to have a high quality of the mesh. Note that in the second phase an unsteady pressure profile will be applied not constant -500 pa.

[Rob]

Have a careful look at the remeshing options: I think you can force a surface remesh which will refine the volume mesh in the constriction. Failing that, search on here as extracting a deformed geometry has been covered before. 

[Jamasp]

Thank you for your reply. 

What remeshing options do you recommend me to use? 

How can I force the surface remesh? Do you mean Local face option? I tried that but didn't help. Maybe I should use appropriate parameters for the interface.

 

I also tried to export the geometry and remesh it in Ansys Meshing but I got errors. Could you please share the link that covers this?

 

Thanks,

[Rob]

I tend to remesh in Fluent Meshing, but also don't have a facet limit: when looking at a mesh in the geometry tools each facet counts as a surface and the Teaching/Student version has a limit of 300. 

From memory (I don't use MDM very much as I can generally work on "if it moves it's failed" for my models) there are some size function settings which should help the meshing. 

[peteroznewman]

You can export an STL file of the deformed shape from Mechanical.  Here is a post discussing the options for using that file in a subsequent model.

[Jamasp]

Thank you for the link. I tried both approaches that you provided on my model. FE Modeler failed to create Parasolid. How can I do this for the fluid domain? My main concern is the quality of the mesh in the fluid domain.

[Jamasp]

We have ANSYS Academic Reseach license. Does it have a facet limit? 

Is there any other way except exporting the deformed model to generate a new mesh for the fluid domain in Fluent? Imagine we have a rigid body in fluid domain can we solve the case with an initial mesh and then after it finishes, continue the simulation with an entirely new mesh?

Thanks,

[Rob]

Research doesn't have a cell/surface cap but you may need a fair bit of RAM if the facet count gets high. 

If it's rigid body motion (ie just a part moving without bending) then you can use the deforming mesh tools in Fluent. FSI is only really needed for when things change shape.  

[Jamasp]

The original problem that I have is FSI but I simplified it. The only thing that I'm looking for is to generate completely a new mesh for the fluid domain in the second phase of the simulation. 

Remeshing tool works for one case but is not for another.

[Rob]

In which case export the surface of interest as an stl and read it into SpaceClaim. I think you'll be OK to read it in as faceted but you may need to do some work before you can export it to Fluent Meshing. 

[Jamasp]

How can I export the surfaces in Fluent?

[Jamasp]

I usually use .cas file and import it to Fintie Element Modeler and then convert it to Parasolid. But for complex geometries, FE Modeler fails to create the model. Is there a better way to do that?

[Rob]

Read the case file into Fluent Meshing. Clear the volume mesh, and you're left with the surface mesh. You'll then need to wrap/remesh the surfaces and generate a volume mesh: probably without the benefits of the Workflow tools. 

[Jamasp]

Thank you for the instruction. I can remesh the deformed model now to use it for the second phase of the simulation. How can I keep the data from the previous simulation? I mean the data from the last time step of the first phase and just remesh it. Is this possible?

[Rob]

Interpolation: write the interpolated file out of the old model & then read it back onto the new mesh.  If you read the new mesh into the old case file it'll also retain the settings on the new mesh: it's the equivalent of the old boundary conditions file from v6.   The interpolation file contains limited data along with x, y, z position which tends to be good enough in most cases. 

[Jamasp]

Thank you Rwoolhou. It worked. I was able to update the mesh for the second phase in an FSI simulation. To summarize, there are three things that need to be done prior to run the second phase of the simulation. Import the updated mesh, read the interpolation file and also read the setting of the old solution.

Useful links: