Fluent Dynamic Mesh not remeshing or layering

  • 1.5K Views
  • Last Post 02 May 2020
ansysuser posted this 11 May 2019

Hello,

I have a 3D FSI simulation which is an elastic cup that deforms by contraction to drive a flow.  I have been able to get the 2D version to work, but the 3D version does not seem to function.  I am using the dynamic mesh with smoothing, layering and remeshing, but I do not see any of that happening. I have tried:

In Smoothing:

  • Springs with Spring Constant 0 and Convergence Tolerance 0.001 for All Elements
  • Diffusion with boundary-distance and Diffusion Parameter 0.1
  • Linearly Elastic Solid  with Poisson's ratio 0.25 and also 0.35

In Layering:

  • Height Based with Split Factor 0.4 and Collapse Factor 0.1

In Remeshing:

  • Local Cell, Local Face, Region Face with Minimum Length Scale set to 0, Max to 0.002
  • Also I tried CutCell Zone on and off.

In the Dynamic Mesh I have the boundary as System Coupling with Cell Height 0.001. I also have the fluid_body as Deforming with Remeshing and Smoothing enabled.

My mesh has a Body Size Function on the elements so that they are tetrahedrons of size 0.001.

The problem is every single combination of these produces results like those shown in the gif - there is no change no matter which of the various settings I have tried.  All of the combinations produce results that look just like these.  I have highlighted several nodes for consideration.  Notice that there is no remeshing, no internal movement, nothing happens to the internal nodes at all. Shown is the symmetry plane as assigned in Fluent, and the solution up to the point of error.  I need to continue the deformation much further past this point, but the Negative Cell Volume error keeps stopping the solution.

 

 

Questions:

 

1. I am getting a negative cell volume error.  What should I look to change in order to get some kind of response from the Mesh Methods settings?  Right now none of them seem to have ANY effect whatsoever.

2. What is the difference between interior-fluid_body (interior, id=1) and fluid_body (fluid, id =4) in my model tree.  Should I be setting the deforming to one or the other or both??  When I try to use the Graphics>Mesh I cannot plot the mesh for fluid_body or fsi_fluent.  Why?

 

 

 

 

 Thanks!

 

  • Liked by
  • mskr
Order By: Standard | Newest | Votes
ansysuser posted this 15 May 2019

Any input at all would help. 

 

What do I have to do to make this model actually remesh??

ansysuser posted this 15 May 2019

More information.  I see this message in the Fluent output file.  Maybe this is why there is no remeshing?

Updating mesh at time level N...
Warning: found cell of wrong type, skip region remeshing on zone 4 at base zone 14.
Warning: found cell of wrong type, skip region remeshing on zone 4 at base zone 14.

 

Any input on what this means?  What is the "right type" and what is the "wrong type" of cell?

ansysuser posted this 15 May 2019

Another finding.  Every single time I try some other setting and re-run this, I find that the Maximum Length Scale has reset and is boxed in red.  Every single time, I copy and past these values but it resets. 

 

WHY DOES FLUENT SWITCH THE VALUES AND THEN COMPLAIN ABOUT IT??  Is this a bug?

 

ansysuser posted this 15 May 2019

Regarding the last comment, this must be a bug in Fluent.  I just changed these to 0.0001 for minimum and 0.0005 for maximum, then I closed Fluent. Immediately I opened Fluent again and the numbers were switched and the red box is back.

 

 

 

ansysuser posted this 16 May 2019

Still need some input.

ANSYSbeginner posted this 17 May 2019

Sorry to hear nobody is helping.  Have you tried cfd-online?

  • Liked by
  • ansysuser
Kremella posted this 17 May 2019

Hello,

My sincere apologies for the delayed response.

Couple of quick thoughts -

  • Have you tried to apply one setting (smoothing, layering, and remeshing - in this order) at a time to understand what might be causing this issue? Perhaps, this will help you isolate the issue. If you've already tried, could you please help me understand the results?
  • Currently, it seems like it is not remeshing at all. You seem to be defining both region and local methods.
  • Could you please share the remeshing settings under 'Mesh Methods Settings dialog box so we can understand it better? I'm looking for the Parameters you might have used. This might also help us understand the 'switch values' issue you are facing?

Regarding your question on interior-fluid_body (interior, id=1) and fluid_body (fluid, id =4): interior-fluid_body is a face zone and fluid_body is a cell-zone. Think of it as surface and volume regions. You can right-click on each and hit display to understand the difference better.

Again, apologies for the delayed response. Looking forward to your responses.

Thank you.

Best Regards,

Karthik

  • Liked by
  • ansysuser
ansysuser posted this 17 May 2019

Hello Kremella,

 

I appreciate your attention - thank you!

  • I have begun the process of trying to isolate the issue.  I have not seen any changes yet, but I will most certainly post updates even if I figure this out so that others may learn from my mistakes/discoveries. :-)
  • It is definitely not re-meshing at all.  I see the cell count every time it writes a solution file, and they are always the same. I am defining both local and region methods.  Is this not preferred?  Should I choose one or the other only?  If so, it would be a great feature enhancement for ANSYS to make these choices exclusive to each other.
  • The 'Mesh Methods Settings dialog' is shown below.  Though in another post I was informed that I don't necessarily have to set the interior_fluid_body as a deforming zone because it should be taken care of when I set the fluid_body as a deforming zone.  Is this correct? If so, that might help me to understand why I kept getting those warnings and why the values were switching. 
  • Thanks for the tip about right-click>Display.  I had not known about that one!  So would it be fair to say that the interior-fluid_body face zone is made up of the faces that are the faces of the cells in the fluid_body cell zone but that are not also part of the exterior (fsi_fluent) boundary?  That is what it looks like.  I am not sure why Fluent needs this zone in addition to the cell zone, but I will look in the documentation to try to understand.

Since I asked my questions above, I have changed the mesh to Cartesian Fitted in my searches for the answer to the problem, so things look a bit different but I will try to document as thoroughly as I can.  As I said, I have tried so many combinations of large elements, small elements, large and small values for the re-meshing length scales and none of them have made any layering or re-meshing happen.

 

 

 

 

ansysuser posted this 17 May 2019

Here are images of the zones of interest for the deforming mesh problem, for completeness.

ansysuser posted this 17 May 2019

Update:  I did get this to run for 20 time steps by taking the interior-fluid_body out of the dynamic mesh, but there is still no layering or re-meshing taking place that I can see.  I need to go to 100 time steps and I am afraid this will fail again without those two things.

 

Here is a gif to show how there is no layering or re-meshing happening, though it does look like the smoothing is effective.

Also, another concern has appeared.  As the solid zone contracts, which drives the flow, I notice that the corner of the fluid zone is getting distorted.  The solid structural zone is supposed to slide there and the fluid zone should move with it but it looks from the image as if it is penetrating the solid.  This can also be seen in the gif.

 

So here is where I am at:

 

Resolved:

Smoothing seems to be working.

Still needing addressed: 

Why is the fluid domain not re-meshing and or layering?  Has it just not gone far enough into the simulation to warrant these things?  I will run it for the rest of the time steps to see if this is the case - i.e. to see if I get a 'Negative Cell Volume' error.

What is going on with that distorted/pinched corner in the fluid domain?  Basically every portion of the boundary between fluid and solid I have set as part of the fsi_fluent zone which is coupled to the structural and so it should deform as needed - I would think.

 

Thank you!

Steve posted this 20 May 2019

Hi there,

Some general thoughts first: If the mesh motion is small enough such that the mesh can deform with only Smoothing, then Remeshing isn't needed. When the mesh motion is large, Smoothing and Remeshing are needed. In 3D remeshing only works on tetrahedral elements. Layering is only used for cylinder-like applications like an IC engine.

It looks like your mesh is hex elements, so that's why you're not seeing Remeshing. It doesn't look like your geometry is a compressing cylinder, so you can leave Layering off. I recommend reading over the following three sections of the help document to get a better understanding of all the Smoothing, Remeshing, and Layering options.

https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v194/flu_ug/flu_ug_dynam_mesh_update.html

11.6.2.1. Smoothing Methods

11.6.2.2. Dynamic Layering

11.6.2.3. Remeshing Methods

Lastly, for FSI cases, it is strongly recommended to perform a simplified analysis with each solver independently before moving to a full 2 way coupled simulation. This will allow you to debug any issues in one solver that are independent of the other solver. In Mechanical, this would mean estimating fluid forces and applying them as boundary conditions. In Fluent, this would mean estimating deformation and applying a moving boundary with a profile, or using a 1way coupled simulation to get the deformations from Mechanical.

All the best with your simulations.

Steve

  • Liked by
  • ansysuser
  • mskr
ansysuser posted this 20 May 2019

 Hello, Steve.

I appreciate your input!  I initially did have tetrahedrons (as you can see from my first post), but I thought I saw somewhere in the documentation that re-meshing only worked for hexahedral elements, and that is why I switched.  I must have misread.  I have already done the simplified analysis for each of the fluid and structural solvers independently, and they were working fine, but I appreciate the reminder.  I will consider the issues about layering and remeshing to be solved, or at least postponed for now.

Do you have any ideas about the pinched corner where the structural mesh slides, from my last reply?

 

Thanks again.

 

 

mskr posted this 02 May 2020

Hey @ansysuser sorry to jump in without helping, but I have a question which I would have asked via DM if this forum supported it. I like your animations. How did you view the motion of the dynamic mesh in Fluent? I have a solution of an FSI case, but cannot see the resulting motion (I posted here https://studentcommunity.ansys.com/thread/cannot-visualize-fluent-dynamic-mesh/). Can you observe it already during solving or only via post-processing?

Close