Divergence detected in IAC for Multiphase Flow

  • 28 Views
  • Last Post 1 weeks ago
  • Topic Is Solved
farizanluthfi posted this 3 weeks ago

Dear fellow researcher,

I have some problems when I try to run boiling heat transfer especially using RPI wall boiling model. My model is helically coiled tubes with the inlet that has been fully developed profile by using single-phase flow then proceed with the boiling model with RPI wall concept. I choose this term because it said in FLUENT it is the best method to capture the boiling near the wall. On this case, my goal is to understand the behavior of subcooled boiling heat transfer in the domain.

But I have got the problems on the IAC (interfacial area concentration) and this parameter got diverged at the iteration more than 1000. Please provide me some resource to troubleshoot this particular problem.

FYI, I am running the simulation with steady-state solver.

Thanks,

Best Regards,

Luthfi Ady Farizan Haryoko

Order By: Standard | Newest | Votes
abenhadj posted this 3 weeks ago

Do not use IAC. Just stick to the default boiling diameter.

Best regards,

Amine

farizanluthfi posted this 3 weeks ago

Dear Amine,

Do you have any idea why we just put on the default setting? Because when I try to read in the manual, it seems like much give you more information about bubble diameter.

Thank you for your kindly support. I do appreciate a lot.

Best regards,

Luthfi Ady Farizan Haryoko

abenhadj posted this 3 weeks ago

Just use the boiling diameter as it is accounting for regime blending. Please use the most actual ANSYS Fluent releases.

Best regards,

Amine

farizanluthfi posted this 3 weeks ago

Highly appreciated for your support Amine, right now I have changed the setup for running my case. Also, I turn my pressure-velocity coupling from coupled into coupled with volume fraction (full multiphase coupled). And my URF I have been changed from the default one.

Is that possible for running my case? Thank you

Best Regards,

Luthfi Ady Farizan Haryoko

abenhadj posted this 3 weeks ago

Yes sounds fine. But again do not use IAC.

Best regards,

Amine

farizanluthfi posted this 3 weeks ago

I have tried for different scheme start with multiphase coupled and full multiphase coupled with different initialization (inlet and hybrid initialization). Also I have changed my URF from default one still got diverged.

Divergence detected for pressure coupled if I use inlet initialization, but I have a different diverged story if I use hybrid init which is divergence detected for vof-1.

Could you please give me some tips and trick for solving this issue? I'm kind of frustrated for find out on what's the serious problem of my case? Your support is much appreciated.

Thank you,

Best Regards,

Luthfi Ady Farizan Haryoko

abenhadj posted this 3 weeks ago

Reduce URF's and try to be very conservative for the first 2000-3000 iterations. I can judge any other settings without pasting screenshots here.

Best regards,

Amine

farizanluthfi posted this 3 weeks ago

I have tried to be very conservative at the beginning of my iterations but it doesn't works, mostly for only 100 iterations will get diverged. Alright, I will give you some screenshots here after this post. Highly appreciated for your concern.

Thank you,

Best Regards,

Luthfi Ady Farizan Haryoko

farizanluthfi posted this 3 weeks ago

Dear Amine,

Could you please send me your email? Because I have reached a limit for posting some images here in this forum so I guess it much better if I could go directly send you through email. 

Highly apologize for the inconvenience.

Thanks.

Best Regards,

Luthfi Ady Farizan Haryoko

abenhadj posted this 3 weeks ago

I apologize but as ANSYS Stuff I can just help on this community.

Best regards,

Amine

farizanluthfi posted this 3 weeks ago

https://drive.google.com/file/d/1Mlv0zs3mHG3ehHU_6xwkBUNlATEgbsIO/view?usp=sharing

Please kindly check the link above, I have attached some pics regarding my problem for subcooled boiling heat transfer. Basically, I do the simulation with multiphase coupled. But I have tried with full multiphase coupled with the same setup in the link above.

Thank you.

Best Regards,

Luthfi Ady Farizan Haryoko

abenhadj posted this 3 weeks ago

AS ANSYS Stuff I would not check the link. Attach your screenshot here.

Best regards,

Amine

abenhadj posted this 2 weeks ago

Switch only drag on at first stage.

Use Tomiyama for lift. Discard virtual mass force and wall lubrication.

Ramp heat flux gradually.

Provide the right operating density.

And use the most actual release.

Ensure that you hace coarse near wall mesh.

Ensure that RPI is the appropriate method (not pool boiling)

Boiling is by far the most complicated multiphase  simulation one can run. You need to be patient.

Best regards,

Amine

farizanluthfi posted this 2 weeks ago

Thank you for your kindly support and attention. I will let you know for the updates of my simulation.

Best Regards,

Luthfi Ady Farizan Haryoko

farizanluthfi posted this 1 weeks ago

Dear Amine,

Sorry for re-open the discussion. I would like to ask you, for drag option that you have mentioned several days ago. So what do you mean is I have to switch on the drag until couple of iterations then after that I turned off the drag option.

Is my interpretation correct? Thank you.

Best Regards,

Luthfi Ady Farizan Haryoko

abenhadj posted this 1 weeks ago

Only Drag force at the beginning. Afterwards you can account for dispersion force.

Best regards,

Amine

farizanluthfi posted this 1 weeks ago

Dear Amine,

Let's say I have done my first iterations until 1000 iterations, so after that, I switch off the drag force and enable dispersion force and turbulent interaction?

Am I correct for this way?

Thanks.

Best Regards,

Luthfi Ady Farizan Haryoko

abenhadj posted this 1 weeks ago

No. Drag is the force which is always required. Recommend reading some text books.

Best regards,

Amine

Close