Learning Forum

[farizanluthfi]

Dear Ansys Community,

I have found the method on running the case for forced convection boiling in the helically coiled tube with some amount of meshing elements. Nevertheless, the problems start to come up when I try to increase the meshing to conduct mesh independence test. Unfortunately, the diverged simulation only exist in one of four cases that I want to do the validation with the experimental investigation.

Highly appreciated for your kindly support and response toward this issue. Thank you.

Best Regards,

 

Luthfi

[DrAmine]

Do use fine near wall mesh with RPI. Yplus larger than 30-60 is required. If not possible check time scales.

[farizanluthfi]

Highly appreciated for your kind response.

For fine mesh, the other case is giving the results only that particular case that got diverged. What possibilities that you try to deliver for fine near wall mesh? Because in my opinion, all of the mesh that I have been implemented in the other case who already got the result must be changed as well corresponds with the new mesh setting. Need your suggestion for this unique problem. 

Thank you,

Best Regards,

Luthfi

[DrAmine]

Actually you ditstribute the heat source terms /evap source terms over a cell layer from the wall. That is what is working and this is state of research (my research 2).

You can start disabling all interfacial forces but not drag and under relax vaporization mass. 

[farizanluthfi]

Thank you for your explanation. It is being understood that the heat transfer from outside the domain comes in contact with the wall due to the process of evaporation. 

The interfacial forces are drag, lift, wall lubrication, turbulent dispersion, and turbulent interaction forces, right? So I just need to activate only the drag force based on your recommendation. 

The URF for vaporization mass is already 0.5, is it necessary to decrease again? Thank you.

Best regards,

Luthfi

[DrAmine]

Yes. Either decrease that or use coupled solver with implicit pseudo time marching. Make consistent cases by not changing more than one parameter at same time

[farizanluthfi]

For disabling all interfacial forces except the drag force, based on your experience, how many iterations that we should allow the setting and turn on the others forces afterward?

For your reference, I have used coupled solver but the case is estimated to be under steady-state condition, so if it is needed to change into pseudo transient, what time step that you would suggest for the boiling case in the helical coil?

Highly appreciated for your kind support. Thank you

Best regards,

Luthfi

[farizanluthfi]

Dear Amine,

I have tried my simulation using your recommendation on turning off all of the interphase forces (except drag forces) and also decrease the URF of vaporization mass to 0.4 from the beginning of the case, but I end up with diverged result in 1715 iterations.

Do you know what's the reason of behind this phenomena?

Thank you

Best Regards,

Luthfi

[DrAmine]

Again the grid might still  be the issue.

Please use coupled steady state solver, pseudo-transient.

[farizanluthfi]

Okay Sir, I will let you know afterwards when I get the result for this.

However, for the previous simulation I'm using the parallel solver instead of serial one, do you think that one of the cause beside the grid?

Thank you,

Best regards,

Luthfi

[DrAmine]

No I do not think so. Serial run on single node should be less prone to parallelization issues as it only done on single node.

We still do not have any idea about your case/problem: please add screenshots of mesh, BC's, models etc...

[farizanluthfi]

Okay, so you think that parallel run for this particular boiling case is acceptable and it's not the cause of the diverged result, right?

Alright Sir, please check on the images here, I attached some picture to make you more understand about the case. 

For outer one, it is the solid (stainless-steel), and for inner one, it is the fluid (water-liquid). Also, that's also my BC for the inlet condition (re:inner one). For the square in the middle, it is basically fluid too but I made that one to ease me on creating the mesh in the domain. this is the mesh elements and nodes

  this is the model that I used

this is the heated wall at the outer one with the amount of heat flux

this is the inlet for mixture phase

this is the outlet for mixture phase

this is the inlet for liquid phase

this is the outlet for liquid phase

this is the inlet for vapor phase

this is the outlet for vapor phase

Thank you.

Best regards,

Luthfi

 

 

[DrAmine]

1/Yes. If you are not convinced try both: parallel and serial (if running with relatively newer version: true serial is starting parallel with t0 "O" CPU's)

2/Main settings are missing : the phase interaction.

 

[farizanluthfi]

1/ Well-noted, Sir. Thanks for your recommendation.

2/ Please refer to the attached file below this comments. I have put the phase interaction setting in the model.

Thank you in advance.

Best regards,

Luthfi

[farizanluthfi]

Hello Sir, please kindly support my case. I have supplied you the phase interaction in the model.

Thank you.

Best regards,

Luthfi

[DrAmine]

Be patient: we do not work in the weekends.

Switch off all forces keep drag at first. Then use simonin for dispersion and sato for interaction.

[farizanluthfi]

Thank you for your input, Sir.

So for this case, I should keep running on the coupled solver with pseudo-transient? Using the 0.1 timescale factor, right?

And for the keeping drag force at first, until how many iterations approximately that I could start to turn on the rest of all forces?

As your reference, I have tried with increasing the mesh and try to run with pseudo-transient but I put all the forces on since the beginning of the simulation. I use 0.1 timescale factor for both liquid and solid time scale. On the 10.000 iterations, the simulation is okay. But when I try to change the timescale factor from 0.1 to 1, it suddenly got a floating point exception in the simulation.

Looking forward to your kind response. 

Best regards,

Luthfi

[DrAmine]

Just change only one set of parameters per run to be more consistent.

Coupled solver with pseudo transient is fine. Keep using small time scale at the beginning. You can even use the Coupled solver without pseudo-transient and tune the URF's /CFL.

Once again (my last comment on this) RPIS is generally used on coarse grid and intended for straight vertical pipes /tubes.

[farizanluthfi]

Dear Amine,

I have been running the simulation based on your recommendation using the coupled solver and pseudo-transient method. The simulation is running well until I can get until 20.000 iterations more but there is one question that I need to ask you about it.

Why the solution to my case seems to evolve for each iteration? Is that because of the pseudo-transient method? Because as far as I know, the pseudo transient is more look like steady-state solution only the URF is controlled by each time step that we defined.

Highly appreciated for your kind responses. Thank you.

Best regards,

Luthfi

[DrAmine]

Pseudo transient is a transient time marching approach to solve steady state problems by adding the same diagonal implicit underrelaxation in all cell. Approaching steady state this artificial transient term wiuld vanish.

Please mark this then as solved.