Mesh deformation and aerodynamic damping calcs
 

Hello all,

I am currently working on calculating the aerodynamic damping of the three "vanes" shown in the attached figure of the flow analysis window (CFX 17.0). I am following the procedure outlined in this paper (Note that my geometry is non-rotating and the flow is incompressible):https://www.researchgate.net/publica..._Blade_Damping

In addition, I am referencing the aerodynamic damping calculation of an initially stationary beam here:
https://www.singularityeng.com/singu...icting-damping

Just like in both references, I first calculated the mode shapes of the vanes using ANSYS Mechanical, and then prescribed the normalized displacements to the unsteady CFX simulation. The mesh motion for the vanes is then generated based on the displacements calculated from the modal analysis. All other boundaries are set to a stationary mesh motion, and the unsteady simulation is initialized by a previous steady state run. The mesh is an unstructured, tetrahedral mesh with about 22 million elements. My problem arises about 6 or 7 timesteps into the unsteady run when the solver generously lets me know my mesh has collapsed:
"A negative ELEMENT volume has been detected. This is a fatal error and execution will be terminated. The location of the first negative volume is reported below."

The location of the collapse occurs on the vane "fillets", where the geometry becomes quite complex next to the domain wall (shown by the yellow star in the second attachment). My solution to this was to split the vanes and fillets apart, and only model the mesh motion for the vanes. Upon doing this, my mesh still collapses but this time at the truncated trailing edge shown in the third attachment. I then decreased the maximum vane oscillation amplitude to about 2% of the chord length - still collapsing.

I am looking for some guidance or any information to prevent this error from occurring, as I do not have much experience with mesh deformation. I have also attached the .out file of the most recent run. My guess is it has to do with the mesh, but since time is limited, I wanted to get some other insight before I dive into that. This is my first post, so please let me know if I need to provide any more information. Thanks in advance for your help.

Attachment 77077

Attachment 77078

Attachment 77079

Attachment 77081

Have you looked at how your structural mesh matches your CFD mesh?

It seems there is motion near the base of the blade. If you plot the profile vector, how large is the displacement imposed by the profile at the base ?

If the base is not moving, and the node shared by the vane and the base is moving, it will fail miserably.

Have you mapped the structural profile to the CFD mesh?

Do you have access to more recent version of the software? Mapping and mesh deformation algorithms have improved since the days of R17.

Hope the above helps

Read the FAQ for some overall comments: https://www.cfd-online.com/Wiki/Ansy..._went_wrong.3F

In your case I suspect you will need to use different mesh motion diffusion approaches to get the mesh to not fold. You are using a mesh stiffness proportional to 1/volume^2, so you are making the smaller elements stiffer. You might want to try a factor with wall distance in it or maybe other parameters.

If nothing with displacement diffusion works then you may need to consider dynamic remeshing.

Hello Drew,

Check if decreasing the time step size will cause the folding mesh error occur at a later time point. If it has an effect, then you may need to keep decreasing the size of the time step till when the problem gets obviated.


Dear Glenn,



Is it possible to use this approach to make the near wall element, I mean those that are within the boundary layer (inflation layer) undeformable? May I ask you to please let me know which variable defines the wall distance? Is there any other variable that can be used to control the mesh stiffness based on the skewness or other quality metrics?


Thanks

The variable "Wall Distance" should be available if you are using the SST turbulence model, or any other turbulence model which uses wall distance as an input.

The mesh diffusion stiffness can be set by CEL, so it can be a function of any CEL variable (to my knowledge). So if you have a CEL variable for mesh skew or something like that you could use that. I would be interested to hear if that approach helped.

Dear Glenn,


Thank you very much.


I'll give it a try and will let you know if it worked.

Opaque: Your comments were helpful, thanks. I do have a newer version of ANSYS on my local PC, however I am using my uni's cluster for this particular simulation which has R17.2 installed.

Glenn: These tips were helpful as well, and I will continue to critique my settings as I figure this out. I have tried using the "Wall Distance" variable to make the elements near the wall stiffer. However, an error returns saying that this variable is zero and therefore cannot compute the mesh stiffness value since it is dividing by zero. Note: I am using Menter's SST turbulence model...any ideas why it is returning this error?


Katty: I am trying out a reduced time step size now, thanks for your tip.

Use a limiter inside the CEL function to avoid it going to zero like max(Wall Distance,0.001) or something.



I did a similar study 2 years ago where I had mesh folding at a region which should not have been critical. See the thread here: https://www.cfd-online.com/Forums/cf...t-volumes.html
The issue was resolved by switching the expert parameter meshdisp diffusion scheme to 3. But check first the other hints ghorrocks and Opaque made. The approach of increasing stiffness towards the wall seems quite nice.

Newer releases have an improved mesh stiffness model named Blended Distance and Small Volumes

It combines the distance to a boundary (Boundary Distance variable), and the volume of a control volume to increase the stiffness in certain regions.

There are ways to tweak the Blended distance model, but the defaults should be enough.

Keep in mind that no amount of stiffness or timestep reduction will avoid a negative element if there is some kind of inconsistency between the moving boundary and the surrounding boundaries.

One way to test if the issue is inconsistency around the boundary edges is to set the neighboring boundary (hub/shroud) in your case to Unspecified, i.e. let them move, to alleviate the inconsistency. If it does not fold, you need to check the settings carefully.

Also, as highlighted by AtoHM there are additional tweaks to improve the quality of the mesh deformation solution. For example,

- solve the equation for mesh deformation more tightly than the others (check Solver Control/Equation Class Settings/ and reduce the target values for Mesh Deformation and increase the number of maximum number coefficient loops.
- use of expert parameters (hopefully you do not have to get here)

Thanks AtoHM and Opaque, I will continue to try these suggestions and let you know when I have come to a solution.

BTW Opaque, the stiffness model Blended Distance and Small volumes looks like exactly what I need. It is unfortunate I am restrained to the older R17 for this particular problem. I am wondering if I could write some CEL to mimic this model using the Theory Guide as a reference? This may be unnecessary, as my current run has not returned any errors thus far (knock on wood) when using a stiffness model dependent on the wall distance only.

Your time might be better spent convincing the university to install the latest version of the software. Hopefully your university has a current license, which means they are entitled to have it. Then it is just a matter of convincing them to install the software, which only takes a few minutes and is straight forward. Even a university IT department should be able to handle that :)

Glenn, funny you should mention that - I had a conversation with IT a few weeks back, and they are updating all software on the cluster this month. Unfortunately, I need these results before then.

With that being said, I got it to run perfectly with no folding by switching the mesh stiffness parameter from a factor of (1/Volume of Finite Volumes) to (1/Wall Distance). Thanks for all your help and that goes for everyone else on this thread.

Best regards

Hi Glenn,




Is there any way to have the "wall distance" variable defined for the non-turbulent simulations?

I can use this variable in CFX but its value is equal to zero everywhere.

Not to my knowledge. You might be able to invoke it with some undocumented feature - try ANSYS support.

Thanks for the reply.


I know using the non-turbulent flow (laminar) model, theoretically we can achieve the same results as if we used the turbulent model, if we can use an extremely fine element sizes.


I am now wondering if we can do the reverse of the above-mentioned procedure. I mean is there any way to use a turbulent model and get the same/similar results of the non-turbulent model?

There is a bit more to it than that - it is Direct Numerical Simulation (DNS) and it means you have to resolve all the turbulent length and time scales, right down to the Kolmogorov scales. To do this you need a very fine mesh, but you also need a very low dissipation numerical scheme and a dirty big computer and lots of time on it. Also, only low Reynolds numbers are practical in this approach.

Do you mean you have a laminar flow but you want to model it using a turbulence model? In this case you want a turbulence model which still works when the turbulence intensity approaches zero, and the effect of the turbulence model (which is the turbulent viscosity) approaches zero as the turbulence intensity approaches zero.

This means you can't use an epsilon based turbulence model (k-e, Reynolds Stress + epsilon) as they get divide by zero problems as the turbulence intensity heads to zero. There are low Reynolds number modifications of these which might work, but they are a little contrived in my opinion. A better approach is to use the omega based turbulence models (k-w, SST, Reynolds Stress + omega) as they have no problems at zero turbulence intensity and correctly have the turbulent viscosity approaching zero as the turbulence intensity goes to zero.

So my recommendation is to use the SST turbulence model. If the flow is laminar and you are using SST it will return very low values of turbulence intensity which give essentially zero turbulent viscosity. The results will then be similar to a laminar model. But not identical - there is still additional dissipation in simply the use of a turbulence model, and the numerical approach used in a turbulent model is slightly modified from laminar; so you would not expect them to be identical. The laminar model will be slightly more accurate due to this lower dissipation.

Thanks a lot for your invaluable information.
Your help is greatly appreciated.:)