Boiling Simulation got DIVERGED when running in the coarse mesh

  • 58 Views
  • Last Post 4 weeks ago
  • Topic Is Solved
farizanluthfi posted this 16 October 2019

Dear admin,

Finally, after several trial and error, my simulation is working and giving the result with sufficient value against the experimental value. It seems that the mesh is not the main factor of the boiling model because when I try to use another option with the same mesh, they could give us good results.

Unfortunately, this particular boiling option can't capture the behavior of the boiling inside the domain within low refinement mesh or coarse mesh. Have you any reasonable idea why it could happen for the boiling case?

Thank you,

Best regards,

Luthfi

Order By: Standard | Newest | Votes
rwoolhou posted this 16 October 2019

Have you checked whether the issue is with the formation of the bubbles or their transport into the flow?  

abenhadj posted this 17 October 2019

Coarse resolution near the wall higher resolution in the bulk: these are passpartout. I made boiling runs with yplus around 20 or lower and that was okay for the particular case.

Best regards,

Amine

farizanluthfi posted this 17 October 2019

Dear rwoolhou,

Thank you for your response. Actually, I'm not sure about that, have you any idea on how to check that in fluent? Highly appreciated for your concern and support.

Best regards,

Luthfi

farizanluthfi posted this 17 October 2019

Dear Amine,

Yes, I absolutely agree with that. I made boiling runs with higher mesh near the wall too, unfortunately for lower mesh it always got floating point in the middle of a simulation. Do you have any recommendations for this issue?

Highly appreciated for your support.

Thank you,

Best regards,

Luthfi

rwoolhou posted this 17 October 2019

Careful looking, look for non-physical velocity spikes.  Not something we can easily diagnose without the files, which isn't something we can cover via the community: nonANSYS staff are free to do this. 

 

farizanluthfi posted this 17 October 2019

Dear rwoolhou,

Can you please demonstrate it how to do it? Highly apologize on this matter due the users are still new one on ansys kinds of stuff.

Thank you,

Best regards,

Luthfi

rwoolhou posted this 17 October 2019

No, as I said we're severely limited in how much knowledge we can use/share on here.  Have a look at the results and see if anything looks odd. 

abenhadj posted this 17 October 2019

Check the heat flux partitions as well as report max value of vapor phase velocity and temperature.

Best regards,

Amine

farizanluthfi posted this 18 October 2019

farizanluthfi posted this 18 October 2019

The boiling options for this simulation is RPI wall boiling model (Non-equilibrium) with k-epsilon model and Non-Equilibrium Wall Fn. Here is the phase interaction that I specified for this case:

Drag : Ishii

Lift : Moraga

Wall lubrication : Antal et al

Turb. Dispersion: Lopez de Bertodano

Turb. Interaction: Troshko-Hassan

Heat: Ranz-Marshall

Mass : boiling

Boiling model :

Bubble departure diameter : tolubinski-kostanchuk

Frequency of bubble : cole

Nucleation Site density : lemmert-chawla

Area influence coeff : delvalle-kenning

Use correction model with fixed yplus value 250

Surface tension : specified

Interfacial area: ia-symmetric

For pressure velocity coupling is Coupled with First Order option in all spatial discretization. The way I run the model is by applying the Energy URF at 0.1 and gradually increase until 0.5. Unfortunately, the result is giving that error at floating point like I take a pict in the previous comments.

Any recommendation is highly appreciated. 

Thank you,

Best regards,

Luthfi

 

farizanluthfi posted this 18 October 2019

rwoolhou posted this 18 October 2019

Have a look at the results from about 7500 iterations: what's happening? Also monitor volume fraction of vapour. 

abenhadj posted this 18 October 2019

How does the geo look alike?

Best regards,

Amine

abenhadj posted this 18 October 2019

Switch all forces off, focus only on drag and turb dispersion. The later switch it a bit later and do not use here Lopez et al.

Best regards,

Amine

abenhadj posted this 18 October 2019

Check if buoyancy is well defined and check the void profile in the volume.

Best regards,

Amine

farizanluthfi posted this 18 October 2019

farizanluthfi posted this 18 October 2019

farizanluthfi posted this 18 October 2019

Dear rwoolhou,

Please kindly check the parameters that I took there in the previous comments. Have you any idea on that one why it could be happened?

 

Dear Amine,

Thank you for your reply. I have shown you my geometry for the boiling case, it's a helical coiled tube with 2 turn. The details of the tube is:

inner diameter: 0.00498 m , outer diameter: 0.00603 m , coil diameter: 0.13 m , pitch: 0.0403 m , total length: 0.82 m

For the phase interaction that you mentioned, is it from the beginning of the iterations or how? and for the turb. dispersion, do you have any recommendations that suitable for my case?

The buoyancy that I used is based on the density of the vapor at saturation temperature and for the void profile, I can't specified it due to the floating point at 7800 iterations. Any guidance is highly appreciated on this matter.

Thank you,

Best regards,

Luthfi

rwoolhou posted this 18 October 2019

Look at the flow field: ie plot contours of stuff and see what's going on. 

farizanluthfi posted this 18 October 2019

For the boiling case, I run with steady-state with pressure based. Also I read some forums that for running the boiling, usually they will use UDF part. Do you have any recommendation on the UDF that I have to set up if necessary?

Thank you,

Best regards,

Luthfi

farizanluthfi posted this 18 October 2019

Dear rwoolhou,

Which part that I need to plot contours? Because in my domain, if we choose the fluid part, we can't see the flow field inside the domain. The only way to inspect that is by applying in each plane of every quadrant. 

Thank you,

Best regards,

Luthfi

farizanluthfi posted this 5 weeks ago

Dear Amine,

I have run my simulation using your recommendations for switching off all of the forces, except the drag and turbulent dispersion force. Also, I'm using Burns et al instead of Lopez et al. After the simulation is getting stable, I could use the other forces until I get the mass balance and outlet vapor fraction value is stable enough and get some convergence criteria.

Unfortunately, another problem is rising due to the coarse mesh configurations. I have tried several ways to run the simulation from the interaction forces but still, the simulation is getting the floating-point. The way I run the simulation is the same with your recommendations and the mesh for the model is around 100k elements. Based on that, I would like to ask you some questions regarding the problem that I have encountered with.

1. In the boiling case, is there any minimum or maximum mesh configurations for us to be considered so the simulation could run properly? Especially when we are using the RPI wall boiling model.

2. If there are any such configurations that we need to take into account, please mention how many elements that we should establish in our model? If not, please give us another alternative way to rectify this issue?

Highly appreciated for your kind support and guidance. I am looking forward to your response.

Thank you in advance,

Best regards,

Luthfi

abenhadj posted this 5 weeks ago

1/ only restriction is that you use coarse near wall mesh. 2/RPI is mainly used for vertical forces convection. Any other deployment is questionable.

Best regards,

Amine

farizanluthfi posted this 4 weeks ago

Can you please give me more explanation on the restriction of using coarse near wall mesh when we want to run the boiling case?

For the helical coiled tube, do you have any recommendation for that?

Thank you in advance,

Best regards,

Luthfi

Close