Learning Forum

[harishkamath86]

Hi, I am working on a steady-state two-way FSI analysis on bearing. I am getting errors related to "Update dynamic mesh failed. Negative cell volume detected".

I am using spring-based smoothing with remeshing parameter (used mesh scale info for min and max. length scale) with size remeshing interval of 4 ( decided after going through many online forum)

Under dynamic mesh zone, fluid face which comes in contact with solid face is coupled by "system coupling". How important is "cell Height" under "dynamic mesh zone" and how to calculate it? whether error is also possible because of this since I have unstructured hex mesh

I have tried this multiple time by varying the mesh of the fluid domain but no use.

Also, can change under relaxation factor in "system coupling" since the default value is 1 with RMS factor is 0.01

Kindly help

Thank you

[Karthik Remella]

Hello Moving deforming mesh generally requires a transient solver. Could you please elaborate on the reasons for using a steady solver?
Karthik

[harishkamath86]

: It is assumed that the shaft has attained the steady-state condition. It has been mentioned in literature that the transient analysis is complex and need a lot of computational time

[Karthik Remella]

Hello A few of points:
Attempt remeshing instead of smoothing. Smoothing will try and preserve the cell connectivities as best as possible, which may be tricky depending on the problem you are attempting to solve. For remeshing, you will need an unstructured tetrahedral mesh (3D).
Please attempt to run a transient simulation. Your simulation as well as remeshing may be more robust. Steady-State analysis is generally very very rare and tricky when using dynamic meshing.
Karthik

[harishkamath86]

Sir, one more query. I might be wrong. but please suggest
Since the clearance between shaft and bearing is very small and hence because of this the fluid pressure exerted on the bearing structure is very large. Later, because of these large pressure values, large deformations are observed in the bearing structure and so to accommodate that bearing deformation, the fluid mesh should drastically change. I think because of this negative cell volume is detected? I am just guessing. How can I steadily ramp the generated fluid pressure on the structure rather than apply it suddenly?
is it possible to do CFD analysis first ( partially solve it) and then continue the system coupling (two-way FSI)

[Rob]

If you run the CFD simulation first you can just map the pressure over to Mechanical: in theory bearings should reach an equilibrium and you can do this with a fixed mesh.

[Steve]

Is this a journal bearing analysis? If so, instead of using FSI to solve for the steady state position of the shaft, it is generally better to prescribe the position of the shaft and run several simulations at different shaft positions. For each simulation, calculate the perpendicular forces on the shaft. Then use DesignXplorer or OptiSLang to get a response surface of shaft forces and shaft position, and use this to calculate the shaft position for the desired shaft forces. This does require running more simulations, but the total simulation and debugging time will likely be less than the single FSI simulation which can be numerically unstable.
Steve