[Ashkan Kashani]

Hello,

Simulation description & objective:
The simulation case is shown in Fig.1. The objective is to study the flow structures around and the forces on a partially submerged rectangular body. In a nutshell, I am using the standard free surface homogenous multiphase model to solve the pseudo-2D transient RANS equations plus volume fraction equation on a structured hexahedral mesh. The CCL is also available in the attachment for full details of the model.
Description of the issue:
After a while into the simulation, the solver starts to struggle with converging the volume fraction equation, which, in turn, causes the adaptive timestepping algorithm (set to 3 to 5 coefficient loops per timestep, as recommended) to severely decrease the timestep size. The following is the typical convergence history in one timestep, showing that while the volume fraction equation is the bottleneck, the rest equations have already converged with small RMS residual values even in the first iteration.
================================================== ====================
| Adaptive Timestepping Information |
----------------------------------------------------------------------
| Direction | Ratio | Last Value | Next Value | RMS Co | Max Co |
+----------------+-------+------------+------------+--------+--------+
| Unchanged | 1.000 | 1.0737E-03 | 1.0737E-03 | 1.59 | 32.50 |
+----------------+-------+------------+------------+--------+--------+

================================================== ====================
TIME STEP = 3722 SIMULATION TIME = 1.9092E+01 CPU SECONDS = 3.629E+06
----------------------------------------------------------------------
COEFFICIENT LOOP ITERATION = 1 CPU SECONDS = 3.629E+06
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom-Bulk | 0.88 | 7.1E-06 | 2.2E-03 | 1.5E-02 OK|
| V-Mom-Bulk | 1.00 | 1.4E-06 | 1.7E-04 | 4.0E-02 OK|
| W-Mom-Bulk | 0.00 | 0.0E+00 | 0.0E+00 | 0.0E+00 OK|
| P-Vol | 1.00 | 2.8E-08 | 6.3E-06 | 12.0 5.2E-02 OK|
+----------------------+------+---------+---------+------------------+
| Mass-Water | 1.00 | 1.7E-03 | 2.6E-01 | 10.8 3.4E-08 OK|
+----------------------+------+---------+---------+------------------+
| K-TurbKE-Bulk | 0.99 | 1.1E-05 | 3.3E-03 | 7.8 2.9E-03 OK|
| O-TurbFreq-Bulk | 0.98 | 8.4E-05 | 5.2E-02 | 7.7 8.4E-04 OK|
+----------------------+------+---------+---------+------------------+
----------------------------------------------------------------------
COEFFICIENT LOOP ITERATION = 2 CPU SECONDS = 3.629E+06
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom-Bulk | 0.98 | 6.9E-06 | 2.4E-03 | 2.9E-02 OK|
| V-Mom-Bulk | 1.47 | 2.0E-06 | 7.0E-04 | 3.6E-02 OK|
| W-Mom-Bulk | 0.00 | 0.0E+00 | 0.0E+00 | 0.0E+00 OK|
| P-Vol | 2.03 | 5.8E-08 | 1.1E-05 | 12.0 5.6E-02 OK|
+----------------------+------+---------+---------+------------------+
| Mass-Water | 0.27 | 4.6E-04 | 1.4E-01 | 10.8 1.0E-07 OK|
+----------------------+------+---------+---------+------------------+
| K-TurbKE-Bulk | 0.16 | 1.7E-06 | 6.0E-04 | 14.7 4.9E-02 OK|
| O-TurbFreq-Bulk | 1.61 | 1.4E-04 | 5.5E-02 | 7.7 5.2E-04 OK|
+----------------------+------+---------+---------+------------------+
----------------------------------------------------------------------
COEFFICIENT LOOP ITERATION = 3 CPU SECONDS = 3.629E+06
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom-Bulk | 0.27 | 1.9E-06 | 6.3E-04 | 4.6E-02 OK|
| V-Mom-Bulk | 0.23 | 4.6E-07 | 1.1E-04 | 9.2E-02 OK|
| W-Mom-Bulk | 0.00 | 0.0E+00 | 0.0E+00 | 0.0E+00 OK|
| P-Vol | 0.42 | 2.4E-08 | 3.5E-06 | 12.0 2.4E-02 OK|
+----------------------+------+---------+---------+------------------+
| Mass-Water | 0.39 | 1.8E-04 | 5.9E-02 | 10.7 2.0E-07 OK|
+----------------------+------+---------+---------+------------------+
| K-TurbKE-Bulk | 0.29 | 4.9E-07 | 2.0E-04 | 7.8 9.3E-02 OK|
| O-TurbFreq-Bulk | 0.12 | 1.7E-05 | 7.8E-03 | 7.7 7.4E-04 OK|
+----------------------+------+---------+---------+------------------+
----------------------------------------------------------------------
COEFFICIENT LOOP ITERATION = 4 CPU SECONDS = 3.629E+06
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom-Bulk | 0.39 | 7.3E-07 | 2.5E-04 | 5.4E-02 OK|
| V-Mom-Bulk | 0.46 | 2.1E-07 | 9.0E-05 | 1.1E-01 ok|
| W-Mom-Bulk | 0.00 | 0.0E+00 | 0.0E+00 | 0.0E+00 OK|
| P-Vol | 0.44 | 1.1E-08 | 1.7E-06 | 12.0 1.7E-02 OK|
+----------------------+------+---------+---------+------------------+
| Mass-Water | 0.51 | 9.1E-05 | 2.5E-02 | 10.8 2.5E-07 OK|
+----------------------+------+---------+---------+------------------+
| K-TurbKE-Bulk | 0.48 | 2.4E-07 | 1.0E-04 | 7.8 9.9E-02 OK|
| O-TurbFreq-Bulk | 0.35 | 5.9E-06 | 2.0E-03 | 7.7 6.5E-04 OK|
+----------------------+------+---------+---------+------------------+

Given the long simulation time required to reach a statistically convergent solution, the small timestep size makes it impossible to achieve the simulation goal. Note that I do not want to study these bubbles, nor do I think they have any considerable impact on the variables of interest.

My suspicion:
In the post-processing, I have noticed tiny air bubbles that are probably entrained at the body leading edge and carried underneath the body. As shown in Fig.2, the locations of these bubbles coincide well with the locations of high residuals corresponding to the volume fraction equation. That's why I think the bubbles are responsible for slowing down the convergence.

Questions:
1- Is my suspicion legit?
2- How to fix the issue? Should I set the timestep manually and ignore the residuals of the volume fraction equation?
3- Alternatively, I have considered to artificially reduce the air density so as to prevent air entrainment in the first place. Does that make sense? I am not sure if this would make any undesired side effect on the simulation results.

I appreciate your viewpoints.

Regards,
Armin

[ghorrocks]

My answers:
1) Probably, yes.
2) If you run a larger time step the VF equation is likely to give rubbish results and possibly diverge. So increasing the time step size is not recommended.
3) Yes, that can help as long as the change does not signficantly change results of importance.

Other comments:
* I see you do not have the surface tension model activated. This would make this run even slower and harder to converge.
* What is the size of this object, and how fast is it moving?
* Do you expect air to be entrained around it in the actual device?
* Can you show your mesh density and quality? VF equations can eb very sensitive to mesh quality.

[Ashkan Kashani]

Dear Ghorrocks, thank you very much for your comments.

Originally Posted by ghorrocks

1) Probably, yes.

I agree with you. An additional piece of supporting evidence is the fact that when I alter a result file by overwriting the variable "Water.Volume Fraction" so as to manually remove these bubbles, and then use that file to initialize the simulation, the volume fraction equation converges much faster without restricting the timestep size.

Originally Posted by ghorrocks

2) If you run a larger time step the VF equation is likely to give rubbish results and possibly diverge. So increasing the time step size is not recommended.

I was hoping that increasing the timestep would only affect these seemingly insignificant air bubbles. Based on your answer, there is no guarantee it is the case.

Originally Posted by ghorrocks

* I see you do not have the surface tension model activated. This would make this run even slower and harder to converge.

As far as I understand, the surface tension model imposes very strict requirements on the mesh as well as the timestep size. I was hoping to evade such requirements as much as possible.

Originally Posted by ghorrocks

* What is the size of this object, and how fast is it moving?

The body is not moving. Please see Fig.1 in the attachment for a sketch of the body and the domain sizes. Note the aspect ratio of the body (i.e. ) ranges from 1 to 30 in my simulation cases.

Originally Posted by ghorrocks

* Do you expect air to be entrained around it in the actual device?

I have not observed the physical experiments myself, but I was advised of no bubble observation by the lab operator. As a result, these bubbles could be a byproduct of imperfect numerical modelling.

Originally Posted by ghorrocks

* Can you show your mesh density and quality? VF equations can eb very sensitive to mesh quality.

Please see Fig.2 in the attachment.

I really appreciate your help.

Regards,
Armin

[ghorrocks]

You have a big jump in mesh size at the front edge of the body, and the aspect ratio of the elements below the body is pretty high (for a volume fraction equation). I would remesh this with 1:1 aspect ratio elements, and larger than you current have. I would then do a mesh sensitivity check to work out what size elements you need.

I think you will find the volume fraction equation will be MUCH better behaved when you resolve these mesh issues, and then the auto time stepping will work fine.

[Ashkan Kashani]

Thank you for your comment.

Originally Posted by ghorrocks

and the aspect ratio of the elements below the body is pretty high (for a volume fraction equation).

I have seen somewhere in the ANSYS documentation saying that the free surface region could be resolved with the inflation mesh (prism cells with high aspect ratio). Why aren't high aspect ratio cells a problem in that case?

Originally Posted by ghorrocks

I would remesh this with 1:1 aspect ratio elements, and larger than you current have.

Since I am using a cartesian mesh, these high aspect ratio cells are inevitable and 1:1 cells are not possible everywhere in the domain (particularly as a result of the inflation layer around the body coming off the walls and going into the flow). Right? So what region(s) of the domain should be covered with 1:1 cells in your opinion? For what regions high aspect ratio cells are allowed here?

Regards,
Armin

[ghorrocks]

I have done a lot of free surface modelling with surface tension, and to get accurate surface tension results you need aspect ratio 1 cells (you get significant deviations even at aspect ratio = 1.2). But you do not have surface tension so your requirements will not be as strict as this, but still I would not push it too far. The surface reconstruction algorithm will definitely work better as the aspect ratio nears 1.

I do not know what aspect ratio is the limit in your case. You are going to have to do the checks to work that out. But the aspect ratio you current have is much bigger than I would use for that model.