[Luk_Fiz]

Hi all (after a long absence

I know that such issue was discussed here but in most cases something more was known. In this situation I have no clue.
Brief description of the problem to calculate:
- FSI (Workbench/CFX) of underwater riser - basically a thin walled steel tube, 100m long, clamped vertically in 1m/s cross flow of water,
- the time scale of things taking place is in range of less than 1s (vortex shedding ~1Hz and so on - not going into details),
- idea is to study influence of viv on structure in time period ~100s.

The problem is, that does not depending on sim configuration (boundary condition, water velocity, turbulence level, mesh) I am not able to conduct calculations for longer than ~10s (this time period is not constant). After few tens of iteration steps the error "cfx exited with return code 1" appears in output and all crashes.
My problem is, that there is no more details given - no negative volumes, convergence problems, nothing, just this "code 1". The only thing I have noticed is, that this issue seems to be related to mesh motion - it always appears after first set of coefficient loops of each timestep, exactly in the moment when mesh transform should be calculated.

My question is:
- how to study the problem?
- is it possible to examine any "hidden" quantity or output file for more details?
- is it possible to monitor something specific during the run here?

Will be thankful for help,
Luk

[mvoss]

I suppose you are doing a 2-Way FSI study. To give a good advice here you have to provide more information.Please post the full error and check the Ansys.err file. Create a VERY stiff solid part and check if the error is still there (no movement-> no mesh movement->problem is mesh related).
Check ALL balances during the run. Create a monitor point on the "maxVal(Total Mesh Displacment)@tube". Also check the max and min angle during the simulation. Is the FEM part convergent? If so, how fast?How tight is the FSI convergence? How many stagger iterations? Did you apply relaxation? If so, for which directions? Puh,...

[Luk_Fiz]

Thanks for Your answer,
At first - I apologize for some of my questions that could seem to be funny but despite I have quite significant experience in fluid dynamics it is one of my first challenges involving solid calculations. Anyway I will try to answer some of Your questions:
1. Yes, it is 2 way FSI,
2. The problem is related to "FSI". When I was trying nonmoving pipe/immersed body pipe (moving-but-not-deforming) it was not occuring,
3. Imbalances are monitored and for me they are not dubious. The possible issue here is, that to speed up calculations I am using (too) rough mesh for fluid, which I know is not going to give right solution. Solid mesh is good, solution of nonFSI case (for example pipe under constant force) is mesh independent, agrees with hand calculations and so on. Total Mesh Deflection is monitored also but does not represent any dubious behavior, up to the point of crash.
4. What angles (mesh) do You mean?

And here we comes to the next point: convergence of solid calculation.
I was able to perform 2 calculations.

A) First one, has limit of 6 coupling iterations setup on CFX. I have noticed that the convergence of solid parts was poor. The calculation crashes as before and output and ansys.err files are as below:

.
.
.
*** WARNING *** SUPPRESSED MESSAGE CP = 17225.328 TIME= 19:57:03
Material number 3 (used by element 16627 ) should normally have at
least one MP or one TB type command associated with it. Output of
energy by material may not be available.

*** WARNING *** SUPPRESSED MESSAGE CP = 17309.516 TIME= 19:57:58
Error in getting field convergence info. From process CFX.

*** ERROR *** SUPPRESSED MESSAGE CP = 17309.516 TIME= 19:57:58
Error during get field convergence Write Please send the data leading
to this operation to your technical support provider, as this will
allow ANSYS, Inc to improve the program.

*** FATAL *** CP = 17309.531 TIME= 19:57:58
An error has occurred. SIF_GetNextRequest, returned the error
message: Read.

COEFFICIENT LOOP ITERATION = 12 CPU SECONDS = 5.873E+04
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom | 1.03 | 3.7E-03 | 7.3E-02 | 1.0E-02 OK|
| V-Mom | 1.02 | 3.0E-05 | 5.4E-04 | 6.7E-02 OK|
| W-Mom | 1.03 | 3.0E-03 | 6.0E-02 | 1.2E-02 OK|
| P-Mass | 0.94 | 2.5E-05 | 6.3E-04 | 5.6 8.1E-02 OK|
+----------------------+------+---------+---------+------------------+
| K-TurbKE | 1.08 | 2.0E-04 | 7.5E-03 | 6.8 3.7E-03 OK|
| O-TurbFreq | 1.05 | 4.3E-04 | 1.5E-02 | 12.6 2.4E-05 OK|
+----------------------+------+---------+---------+------------------+

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX solver exited with return code 1. No results file |
| has been created. |
+--------------------------------------------------------------------+

End of solution stage.

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| ANSYS Solver terminated with return code 256 |
+--------------------------------------------------------------------+



B) After this, I have shift the limit of stagger iteration to 15. The solid convergence improves, but anyway (for each general timestep) plattoed after about 10. Simulation also crashes but for different reason:

.
.
.
*** FATAL *** CP = 16956.266 TIME= 00:35:18
Error during get surface loads: Total Force. Error Message: Read.

----------------------------------------------------------------------
COEFFICIENT LOOP ITERATION = 31 CPU SECONDS = 5.902E+04
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX solver exited with return code 1. No results file |
| has been created. |
+--------------------------------------------------------------------+

End of solution stage.

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| ANSYS Solver terminated with return code 3840 |
+--------------------------------------------------------------------+



So it seems that something is around here.

[mvoss]

Make sure to reach convergence on the fluid-side (RMS 1E-5 - MAX 1E-03 e.g with sufficient Coeff.Loop Iterations e.g. 15) in every Stagger Iteration. Tighten up the mesh movement calc. (at least RMS 1e-6) in CFX with sufficient iterations (10-15 e.g.).
Did you reach convergence in the ANSYS Interface Loads (Structural) for every Coupling Step up to the error?
Monitor the Interface Forces WITHIN the Stagger Iteration.

[Luk_Fiz]

Thanks for kind help,

To Your questions:
1. I will try to achieve such tight tolerances (by curiosity: why that tight? Reaching down to 10^-6 seems quite unusual for me, in general I mean).
2. No. The before the crash, for every external timestep, solid platoed after ~10 (of allowable 15) iterations. Observing residuals, imbalances etc. there is nothing really happen just before calculation crashes (in any runs not just the last one).

In the morning I have started the same calculation but with timestep decreased 3 times, dont know results yet. By the way: is it possible to setup for FSI something like autotimestepping, or ranges for which solid solver can move with timestep? (FSI tutorial says that it is only possible to setup timestep for stiff, both for CFX and Mechanical - in CFX Analysis Option window).

Luk

[mvoss]

Originally Posted by Luk_Fiz

Reaching down to 10^-6 seems quite unusual for me, in general I mean).

how do you know? Especially the mesh movement is crucial.

Originally Posted by Luk_Fiz

2. No. The before the crash, for every external timestep, solid platoed after ~10 (of allowable 15) iterations.

What do you mean by "platoed"? Afaik the FSI convergence should decrease aslong as you apply more fsi iterations - resultung in a zig-zag-shaped curved for ALL forces and moments.

Originally Posted by Luk_Fiz

In the morning I have started the same calculation but with timestep decreased 3 times, dont know results yet.

This could help but also increase the chance of getting the "virtual added mass"-effect to kick in. Which by the way could be of interest in your case if you have a low density ration between solid and fluid and have lot of fluid moved by the structural part.

Originally Posted by Luk_Fiz

By the way: is it possible to setup for FSI something like autotimestepping, or ranges for which solid solver can move with timestep? (FSI tutorial says that it is only possible to setup timestep for stiff, both for CFX and Mechanical - in CFX Analysis Option window).

Afaik this is true, CFD and FEM must have the same timestep. Maybe in the next release.
Did you apply any relaxation?

[Luk_Fiz]

Hi,
At first - decrease of timestep does not change anything, crash occures again for the same reason (.err file).

By plateau - I mean within one external loop. Convergence plot is peaky indeed, but decreases rapidly through first 7-9 coupling steps (from 15 set up for last tests). Afterwards, there is plateau and peak again of the start of next external loop.

What do You mean by relaxation? Underrelaxation of CFX params. Yes I did - 0.5 for all that "exported" - forces and translations.

Ok, I will try to beat down the residua.

Luk

[Luk_Fiz]

Hi all,
I want to add, that trying to solve a problem while 2 days I have noticed another error in Ansys.err file stating that (from my memory, have not direct system output): "unable to get convergence data from cfxsolve". Observing convergence plot, nothing serious happened.

I was able to improve a bit convergence, but not to the suggested range ~10^-6. Problem is still unsolved.

Luk