[Turbomachine]

Dear All,

I am encountering negative volumes when running a mesh deformation problem for a compressor blade. The negative volumes occur near the blade tip at the leading edge, where the deformations are the largest and most rapid.

The mesh motion is set to specified displacement for the blade, conservative interface flux for the shroud tip (with GGI connection) and the shroud is set to unspecified.

I tried varying the mesh stiffness exponent and coarsening the mesh both without any effect and also changing the mesh itself. The first mesh is a HCJO grid the second one an elliptically smoothed mesh done by ATP. I haven't considered remeshing yet because the deformations are not too significant and also because I am not sure about this area.

Can anyone help me out?


http://picasaweb.google.com/11157939...35640474701842

http://picasaweb.google.com/11157939...35922577220562

http://picasaweb.google.com/11157939...35636769441554

[ghorrocks]

I was not aware that you could do moving mesh and rotating frames of reference at the same time. Just a check - you are using rotating frames of reference for the rotation, and moving mesh just for the small blade flexing, aren't you (ie, not using moving mesh to define the rotating motion)?

Can you describe the sort of motion you are modelling? Is it in one direction only? Or is it a complex flexing motion? Or a AOA change or something else?

[Turbomachine]

Dear Glenn,

This procedure is a part of an aeroelasticity analysis of a fan blade. One major assumption I use is that the feedback from fluid pressure forces to the structural solver is negligible, therefore one way coupling is sufficient which is often the case.

I have therefore done a modal analysis to determine the modal shapes and the natural frequency. Instability is most likely to occur at this frequency, hence what I am interested in is the blade transient pressure distribution while the blades are vibrating in a particular mode. This is a trial I made recently.

http://www.youtube.com/watch?v=2iUjqVK20H0

This is a linearly varying displacement much less sophisticated than a fan blade but the idea is the same.

My currently problem is that the blade tip s undergo the most severe amplitudes ans vibration rates therefore the mesh usually produces negative volumes there. I have now divided one cycle into more timesteps (100) so there is more time for the solver to smooth out the mesh. This seems to help, but I still dont have a working model. I am also trying to make it less refined at the blade tip, which is useful for the deformation but not beneficial for the fluid solution accuracy. Changing the mesh stiffness had no effect whatsoever. Do you know about any other parameters might help avoid negative volumes?

[ghorrocks]

The mesh stiffness is your best bet. Making the stiffness proportional to the inverse of the cell volume is worth a try. If that does not work try making the stiffness proportional to the distance from the blade.

[Turbomachine]

Thanks for your help! Having done a lot of adjustment, I managed to avoid negative volumes in the first cycle. Even stranger now, negative volumes occur now in the second cycle, when the blade is meant to undergo exactly the same deformation as in the first cycle.

How is that possible? As far as I am aware CFX solver does some mesh smoothing operations during deformation. Since the mesh fails in the second cycle, which is identical to the first cycle I suspect the mesh may have changed during that time. If worse come to worst is it possible to load the original mesh every x timestep?

[ghorrocks]

You can "reset" the mesh by interpolating onto a new mesh and starting again. This is a bit crude and it can be done a lot more nicely using the new mesh morphing stuff in CFX V13. If you are still having problems you might consider using the new mesh morphing stuff.

[Turbomachine]

For the first model, whereby the blades move in phase I managed to implement the movement, firstly by setting the mesh stiffness exponent to 1e4 (increase near small volumes). This wasn't enough though and I had to decrease the mesh density at the blade tips where the deformation is the largest.

However for the second case, whereby the blades move opposite to each other negative volumes occur in the boundary layer again. See pictures (first negative volume is marked with a star):





It seems that the mesh distorts significantly at the boundary layer, whereas the distortion is acceptable further away. The rest of the mesh (not shown) would be able to accommodate a lot more distortion, but the latter on concentrates at the blade somehow.

In this case I cannot decrease the mesh density any further. Therefore I have tried changing the mesh stiffness and the settings for the mesh diffusion equations, but it did not work for this case. For the case shown on the picture the values used are:

Mesh stiffness: Increase near small volumes, tried settings from 10-1e10
Mesh diffusion eq. Max coeff. loops 50
Convergence 1e-5

Can anyone suggest an expression for the mesh stiffness such that the stiffness decreases with the circumferential distance from the blade? Any other solution, or suggestion would be highly appreciated.

[singer1812]

Instead of Increase Near Small Volumes, have you tried Increase Near Boundaries?

[Turbomachine]

Thanks for your reply singer1812! Yes, I did try that option as well, however it produced the same results. What I suspect is that since the folded mesh is close to the blade tip (which is where the highest blade deformations occur), which is in turn close to the shroud boundary, the elements may have become stiffer here due to this setting.

Can you give me a clue as to what other option I may have? I have spent a lot of time refining the mesh at appropriate places according to the steady state results. Therefore I'd like to keep as much resolution as possible at the blade tip and at the leading and trailing edges to keep the accuracy of the solution, which made me drop the idea of changing this mesh. In addition, I tried to make it as coarse as possible since it helped to avoid negative volumes in the last run.

Does anyone know a better solution?

[singer1812]

Did you use a stiffness around 1 instead of 10 for near boundaries? 10 is applicable to Buildings...

[Turbomachine]

Did you use a stiffness around 1 instead of 10 for near boundaries? 10 is applicable to Buildings

Can you elaborate on this a bit more?

[felipelang]

Originally Posted by Turbomachine

Dear All,

I am encountering negative volumes when running a mesh deformation problem for a compressor blade. The negative volumes occur near the blade tip at the leading edge, where the deformations are the largest and most rapid.

Turbomachine, did you have any advance in this thread?

I'm dealing with the same problem of folded mesh, but in a plane wing instead. The resulting mesh from deformation has the same problem that yours.

Best regards,

[felipelang]

Originally Posted by felipelang

I'm dealing with the same problem of folded mesh, but in a plane wing instead. The resulting mesh from deformation has the same problem that yours.

Just to make an update on this thread, I solved this problem paying attention to the % of un-matched area on mapping between CFX and Ansys. The ANSYS structural geometry external shape can't be very different of the CFD geometry, at least in my problem. The result of using a very different geometry can be seen at the picture below that shows the upper wing surface and the deformation that lead to folded mesh:

problem1.jpg

However, another error source can be the thickness of the wing trailing edge that may not support the pressure loads. This may result in a large value of displacement, folding the CFD mesh, like in picture below, showing the wing trailing edge.

problem2.jpg

Furthermore, lowering the mesh displacement equations residual target and increasing the number of coefficient loops allowed works in a great number of problems. For me setting the displacement diffusion to "increase near small volumes" was the best, and the coefficient value didn't produce any valuable changes, so I used it 1.