[AtoHM]

Hi all.
I am aware that negative volume occurrence in transient runs has been a frequently asked question. I read most of the threads I found, but could not really find a similar question, so here it goes.

I am conducting a flutter simulation with a single passage turbine blade. It has the first bending modeshape applied, with a max amplitude of 1.3mm at the tip trailing edge. A single vibration cycle is resolved by 80 timesteps. As cfx applies a Sine-displacement, I get the maximum amplitude after 20 steps; it goes down to 0 displacement at step 40 and then it moves to the other direction. The mesh was set up with Turbogrid using the traditional technique, because I need the 1:1 matching interface at the tip. It has at least 20° min. phase angle.
While running, the mesh is displaced, phase angles are stable at 20° and no negative elements occur until and a while after the maximum amplitude. Whoever, a few steps before reaching its original position, I get negative cell volumes. Also, the maximum displacement at the abortion time step is higher than the original peak value, as you can see from the attached images.

To be honest, I do not understand what is going on there. From looking at the displacement plots, I clearly see how the mesh is folded, still, I have no idea why it happens and especially, why it happens after reaching the maximum amplitude.

Any suggestions on how to resolve this? I tried many of the mesh stiffness options and parameter values, they just influence at which time step I get the exact same result.

Images: left, at abortion time step, right at max. amplitude, step 20

[Opaque]

May I ask what release version are you using ?

[AtoHM]

Sure, this is CFX 17.1

[Opaque]

Another question, are you deforming from the Initial Mesh option or Previous Mesh? They behave differently, and for periodic motion, it is always best to use Initial Mesh

[AtoHM]

Yes I chose Initial mesh and applied Periodic Displacement to the blade walls

It seems the compression of the cells is handled differently than the expansion. I wonder if the stiffness used is calculated at each time step or only initially depending on initial volume. If it is updated each time step, that could lead to a stiffness increase at the passage position, which aggravates re-expansion of the cells. However, that should lead to the whole area seen being stiffness-increased rather than those thin lines. The mesh application method seems to have some flaws here, especially if it fails for small amplitudes and works for bigger ones.

[ghorrocks]

This might not help much but I noticed a similar thing in some internal combustion engine modelling I was doing. If you start with the piston at bottom-dead-centre and compress it the mesh is liable to go haywire and fold. If you start the piston at top-dead-centre and expend it it works fine, including running over several engine cycles.

I worked around this by simply starting my models at TDC and going from there, which was the logical place to start my work anyway. But I appreciate this is not possible in all cases.

That work was some time ago, and since then the mesh smoothing algorithm has been significantly improved. You can now constrain nodes to surfaces and the mesh smoothing should be more resistant to going haywire like this. But I must admit I have not played with it in detail, so cannot offer any suggestions other than to just try some of the mesh smoothing options.

[Lance]

I always run my mesh deformation case with the expert parameter
meshdisp diffusion scheme = 3
which forces CFX to use positive definite values for the mesh diffusion equation. I have found that it increases robustness, and might be worth to try for your application too.

[AtoHM]

Originally Posted by Lance

I always run my mesh deformation case with the expert parameter
meshdisp diffusion scheme = 3
which forces CFX to use positive definite values for the mesh diffusion equation. I have found that it increases robustness, and might be worth to try for your application too.

Wow. I added your suggestion and my simulation just ran through the first cycle without changing maximum phase angle more than 0.1 degrees. Also, the mesh displacement residuals are way lower than before, which is a prerequisite for a smooth displacement I guess. I thank you very much, Sir!

@ghorrocks,
unfortunately starting movement in the other direction would not really help, since for flutter with multiple passages I will later on need 2 blades vibrating out of phase, so at least one would move like my previous setup.
I also tried relaxing the mesh motion by unconstraining the interface and shroud mesh motions, but results just seemed to vary randomly.

My whole run consists of 8 cycles, I will update this thread if I experience any further problems so if anyone also experiences something similar in the future, they might find help here.

[Lance]

Originally Posted by AtoHM

Wow. I added your suggestion and my simulation just ran through the first cycle without changing maximum phase angle more than 0.1 degrees. Also, the mesh displacement residuals are way lower than before, which is a prerequisite for a smooth displacement I guess. I thank you very much, Sir!

Im happy to help. Good luck with your simulations.

[AtoHM]

Hi again,
I got a more detailed question about the mesh displacement diffusion scheme. The information provided within the ANSYS guides is a bit distributed and hard for me to understand, so maybe you can help.

Now what I understand is, that CFX needs to solve the diffusion equation for the mesh displacement. As with any other variable, there must be some kind of numerical scheme to do so. From the manual I extracted, that the standard mesh disp diffusion scheme = 2 and uses positive definite coefficients (interior) and "central" at boundaries.
Going for mesh disp diffusion scheme = 3, as you suggested, switches to positive definite values both interior and at boundaries. I can't seem to work out where exactly the positive values are forced? Are those positive coefficients actually the entries in the diffusion tensor (which is denoted mesh stiffness in the guide)?
I am confused because "central" is obviously a numerical scheme, but "positive coefficients" and "positive definite values" aren't (to my knowledge) ... so its mixed up a little. Any help is very much appreciated.

[mrkmrk]

Hi,

Does anyone know about the effect of setting the expert parameter of "meshdisp diffusion scheme"? What changes it makes into the algorithm.

I am performing the FSI simulation on a case study with the value of 4 for this expert parameter and surprisingly I am getting the negative volume element error at a point where there is no element there.

Thanks.