[KeganLeckness]

Hi all,

I'm currently running a conceptual model to decide on a proper mode of pressure initialization for my actual model.

An analysis using this model failed, with the output:

+--------------------------------------------------------------------+
| ERROR #002100012 has occurred in subroutine Out_NegVol. |
| Message: |
| 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. |
| Volume : -0.8408E-08 |
| Location : ( -0.13762E-01, 0.19524E-01, 0.44175E-01) |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #002100012 has occurred in subroutine Out_NegVol. |
| Message: |
| 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. |
| Volume : -0.1531E-06 |
| Location : ( 0.14810E+00, -0.92774E-03, 0.22935E-01) |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| CFX encountered the error: |
| 0. A folded mesh has oc- |
| curred. This process will shut down as soon as possible. |
| |
| |
| |
+--------------------------------------------------------------------+


Going back into CFX-Pre, I used the locations listed above to create Monitor Points so that I could visualize the location of the error, and maybe decide where I need to re-mesh. Upon the creation of the monitor points, I noticed that these locations are well out of any fluid domain.

Is there anyone who knows what is happening here and what I could do to get rid of this problem? An image is attached with monitor points circled.
Thank you,
Kegan

[ghorrocks]

This suggests your equations of motion went haywire (if a moving mesh simulation), or your FEA/CFD coupling was very poor (if a FSI simualtion).

[Lance]

...or that you used the wrong units when creating the monitor points in pre. There are no units in the output message so a change from [m] to [mm] might solve the problem - I had the same issue a couple of weeks ago.

[KeganLeckness]

Lance, I checked and the CFX-Solver output uses SI units and CFX-Pre is also set to meters, so I don't believe this to be the issue. Thank you.

Ghorrocks, this does involve both moving mesh and FSI. I do not believe the issue to involve the FSI, as I've run multiple simulations under slightly different conditions with no issue. The only change resulting in this issue was halving the distance from the inlet (the small hole in the box domain) to the entrance of the cylinder.
Do you have any suggestions of how to fix this problem?

[KeganLeckness]

I'm not sure if my first response will get to you, so this is just to hedge my bets.

Thanks

[ghorrocks]

In that case it is highly likely this is the FSI going unstable and generating wacky deformations. I am no FSI expert so cannot tell you exactly what option to look at but I would try using a smaller time step and/or more accurate FSI coupling.

[KeganLeckness]

Thank you, ghorrocks. I will look into methods for increasing FSI coupling. I have one last question regarding this problem:
I was just able to get this same model to converge when I used structural steel (E=2E+11, dens=7850) instead of the material properties I'm interested in (E=2E+7, dens=1200). I've had a lot of trouble getting CFX to converge when I've made this change; ANSYS handles it fine. I'm having trouble understanding why CFX experiences convergence issues when changing to the more elastic material, unless the issue stems from the fluid elements distorting more (since the solid object gives more). Is this a reasonable conclusion, or are you aware of something else that may make CFX less likely to converge after decreasing a solid's stiffness?

I greatly appreciate your help,
Kegan

[ghorrocks]

It makes absolute sense that less stiff materials will be harder to converge. For a given fluid loading, the less stiff material will deflect more. So that means a less stiff material will require much finer time steps and coupling to handle this stably. You would expect the nodes to fly off into space when it is not stable - and that is exactly what you are seeing.

[quantum mechanic]

One way to avoid folding mesh problems is to allow the mesh to move with as many degrees of freedom as possible, i.e. why have a stationery wall if you can let translate in the plane of the boundary. This will allow the mesh more elasticity during large deformations. increasing the stiffness of the mesh seems to only remedy small displacement mesh folding.