Your hypothesis about increasing pressure in the tank can easily be proven by a monitoring point, where you observe pressure during simulation. This would show such an increasing pressure. Seems like you did this already and a prssure of 150 MPa will most likely keep the water in its liquid state.

Potentially you might want to replace the top wall of the tank with a degassing boundary condition. By that you make the tank an open container being at all time under the specified reference pressure.

Hopefully you have setup the multiphase flow mixture correctly with one phase as IAPWS water in liquid state, the other phase as IAPWS water in gaseous state (vapor) and with a IAPWS homogeneous binary mixture to link both phases together (surface tension and other thermodynamic properties defined at the phasic interface) under the condition of phase change. In addition to the definition of the wall boiling model on the heated wall you need to define a thermal phase change model with appropriate mean (steam) bubble diameter in the bulk fluid in order to characterize the re-condensation of the formed steam bubbles in the bulk fluid properly. This has a great influence on how rapid/fast the recondensation away from the heated wall is taking place.

Looks like the case of heat addition raising the pressure of liquid in a closed container

Dear Thomas Frank , with outlet boundary for the top surface, I had the pressure in the tank under control. Temperature was also increasing with time. But when it approached near to saturation temp. (365-373K), the solver stopped with fatal overflow error (Maybe increased agitation in the tank would have caused backflow at the boundary). Of course I saw too many warnings for overflow for both phases at the end of each iteration and residual plots were also very unstable. But I let the solver continue to solve and generate transient results with time as much as it could.

When I used degassing boundary for the top surface, the pressure surprisingly kept increasing with time. Of course, now I had overflow warnings only for one phase (the liquid) and residuals were also very smooth, but the pressure rise in not understandable. This will never let me see vapor phase in the domain.

I can not even use Opening boundary, as I do not have Opening temperature required for its definition.

What can I do to successfully simulate the multiphase boiling in such case?

P.S.: I did not use Homogeneous binary mixture to link both the phases; I rather defined two separate fluids, 1st one as liquid-Continuous phase and 2nd one being Vapour- Dispersed phase in the domain definition, as per one ANSYS Workshop tutorial on RPI Wall boiling and Thermal Phase Change, where special CEL is used for parameters like BubbleDiam, etc. and where simulation results were compared with Bartalomej test case.

Should I have used the Homogeneous Binary Mixture definition approach?

Difficult to make a good judgement about the correctness of your setup without actually being able to study it. You talked about the Bartolomei setup which you tried to adopt. But with using IAPWS I think that a homogeneous binary mixture object for saturation temperature and surface tension properties is mandatory. Seems like your two phases in the Eulerian MPF setup are not properly linked to each other or the introduced heat is not sufficient to produce vapor or the mesh resolution close to the hot surface is too coarse, so that the produced vapor in the near-wall cell is immidiately condensing again or.... Many possible reasons, why you see what you are observing.

Thank You Dr. Thomas Frank .

I will further refine the mesh. Also, I would introduce the third fluid material as Homogeneous binary mixture defined as (IAPWS) of the two phases (also defined as IAPWS). So, should I use that HBM in the domain definition alone? or should I simply keep it created it in the materials list?

It is sufficient to keep it created in the material list. It is just a construct to tell the solver, that the one material is the gaseous phase of the other liquid material and to contain the thermodynamical properties, which do belong to the interface between the two phases (like surface tension, saturation temperature) and not just to either one of the phases alone (like density, viscosity, etc.).

For wall boiling applications it is recommended to have a first mesh cell layer at approx. y+ between 50 and 30. Too fine mesh refinement near the heated walls lead to very thin mesh cell layer at the heated wall, which does not contain enough liquid anymore in order to convert the wall heat flux into latent heat of evaporation. For such very refined meshes the consequence is solver instability in the wall boiling model. So proper mesh generation for wall boiling applications is a bit of tricky thing... Not too coarse and not too fine.

Thank You Dr. Thomas Frank .

Thank you for giving me hint for meshing as well.

Dear Dr. Thomas Frank , I am now first trying to do proper meshing (hex meshing).

I am assigning appropriate cell height in the tank domain around the tube wall (where RPI wall boiling is assigned) as per your suggested Y plus range.

But what about the cell length? Does the aspect ratio of the meshing quality matter?

Also, should I be consistent with the cell size all over the domains or can the meshing go coarser away from the tube wall?

Thank You.

Usually in or close to boundary layers with ANSYS CFX the higher aspect ratios are not a reason to worry too much. Cells in boundary layers are well aligned with the flow direction, so that interpolation errors due to large aspect ratios are not very present. Aspect ratios as high as 2000-3000 are rather common. But if smaller, than of course better.

The mesh not necessarily needs to be homogeneous with cell sizes. So you can expand with usual expansion factor of

Thank You Dr. Thomas Frank

Dear Dr. Thomas Frank ,

The outlet boundary issue is not bothering anymore after I changed the CEL expression to be used for Mean Diameter of Dispersed Phase Morphology definition for which I have been using CEL expression from Bartalomej test case ANSYS CFX Workshop tutorial.

I probably meshed properly; there are now enough inflation layers 10-15 covering suggested Y plus distance with first cell height also as per Y plus calculation.

So, I think, the problem is with the CEL expression for local/bulk bubble diameter.

Can you please suggest me an appropriate expression?

I already tried the converting the following attached equations into CEL expressions. The one from ANSYS tutorial CEL doesn't make any considerable vapor fraction and rather cause Outlet boundary overflow error while the other one gives error right after a few iterations (solver clearly mentions the Mean Bubble Diameter error) but has not even backflow warnings at the outlet.

Thank You.

What do you mean with an "Outlet Boundary Overflow Error"?. Mentioned recirculation at an outlet is not a matter of concern, as long as this warnign disappears after some flow development. It can be suppressed alltogether by an expert parameter setting in the CFX-Pre GUI, which is what I usually do, since I find this "artificial walls" at outlets rather counterproductive. The expression from the Bartolomei tutorial should work, also the 2 diameters between which the expression blends with a tangens hyperbolicus might need some adjustment for your case. It essentially binds the local bubble diameter to the local liquid subcooling. Close to the heated wall this expression is supposed to deliver a diameter close to the bubble departure diameter. Far from the heated wall it is supposed to go asymptotically to zero due to vapor recondensation in the subcooled liquid. It can be helpful to plot for your case the dependency of this mean bubble diameter over the distance from the heated wall in order to verify, that this expression is doing the right thing for you.

Dear Dr.Thomas Frank,

In my transient simulation, this warning starts with the first iteration (initial temperature conditions in thank) till final iteration (when tank reaches ~90 C) after which solver stops with 'Fatal Overflow Error'. Can I avoid the solver failure by supressing this artificial wall issue by expert parameter?

Also, can you please guide/suggest me any research article to know how to ADJUST and smoothly blend between the two diameter?

The expression is already the smooth blending. Please start your simulation until boiling is occurring and visualize the bubble departure diameter at the wall in CFD-Post. Than plot a mean bubble diameter profile normal to the wall and see, whether it fits exactly this bubble departure diameter at the wall surface. If not, adjust the expression parameters accordingly.

The Fatal overflow error is straight solver divergence. It cannot just be avoided by setting a "magic bullet" expert parameter. Something is still physically wrong in your setup. But from the outside without analyzing your setup deeply it will be almost impossible to give any good advice where to find the issue.

https://www.sciencedirect.com/science/article/.../S030645491300476...

Any one have RPI boiling model tutorial class?