[Mytho]

Hello everybody,


I am currently working on a one-phase simulation using the rhoPimpleFoam solver, but unfortunately, I am encountering issues with the convergence of the pressure field.
The simulation involves a helix tube with the following dimensions: length of 8m and a height of 0.5m. Although the case appears to be relatively straightforward, I am perplexed as to why the convergence is proving to be problematic.
If anyone could lend their expertise to help diagnose the potential sources of error in my setup, I would be incredibly grateful.To aid in the analysis, I have attached the relevant case parameters and an the log file.


Thank you in advance for any assistance you can provide.

[Tobermory]

Wow - your log file is REALLY difficult to read, with all the repeat info ... I am not sure why it is so "polluted". Anyway, here's what I have gathered from a quick skim before my eyes crossed:
- your pressure & velocity boundary conditions seem reasonable, but there again you haven't provided enough info on the problem ...
- your Courant number is acceptably low, so no problem with the time step at first sight
- you have really tied down the pressure field tightly, between 47 and 49bar .... I don't know what the speed of sound is for your fluid to tell whether that's an issue or not ... have you tried widening this?
- you keep hitting the limit on pressure iterations (1000) for each time step which is a sign that the solver is really struggling; the velocity and energy fields solve really easily.

Some basic questions:
- what's your mesh quality like? Did checkMesh run without warnings?
- what sort of Mach numbers are you expecting in the flow? This might affect your choice of boundary conditions. What Ma are you getting? Iy's often a good idea to use the fieldMinMax function object to track the min/max values of p, T, U etc. in the run

Hopefully that will have flushed out some problems for you.

[Yann]

Originally Posted by Tobermory

Wow - your log file is REALLY difficult to read, with all the repeat info ... I am not sure why it is so "polluted".

Mytho started rhoPimpleFoam using mpirun, but he forgot to add the -parallel option for the solver so it started n serial rhoPimpleFoam processes rather than running the solver in parallel mode.

@Mytho, the proper syntax should be something like this:

mpirun -np core-number-you-want-to-use rhoPimpleFoam -parallel

However this won't change the convergence issue, so Tobermory's comments are still on point.

Regards,
Yann

[Mytho]

Originally Posted by Tobermory

Wow - your log file is REALLY difficult to read, with all the repeat info ... I am not sure why it is so "polluted". Anyway, here's what I have gathered from a quick skim before my eyes crossed:
- your pressure & velocity boundary conditions seem reasonable, but there again you haven't provided enough info on the problem ...
- your Courant number is acceptably low, so no problem with the time step at first sight
- you have really tied down the pressure field tightly, between 47 and 49bar .... I don't know what the speed of sound is for your fluid to tell whether that's an issue or not ... have you tried widening this?
- you keep hitting the limit on pressure iterations (1000) for each time step which is a sign that the solver is really struggling; the velocity and energy fields solve really easily.

Some basic questions:
- what's your mesh quality like? Did checkMesh run without warnings?
- what sort of Mach numbers are you expecting in the flow? This might affect your choice of boundary conditions. What Ma are you getting? Iy's often a good idea to use the fieldMinMax function object to track the min/max values of p, T, U etc. in the run

Hopefully that will have flushed out some problems for you.

Hi Tobermory, thank you for your answer,
i had to tie down my pressure cause of the issue regarding the fluctuation of pressure, which deviates significantly from the desired range. My main objective is to simulate a water wall boiling process, where I need to specify a given Heat Flux at the Wall and a specific Mass Rate/Velocity at the inlet. It is crucial that the pressure remains within the range of approximately 4.8MPa.
Initially, I performed a checkMesh, and fortunately, all aspects seemed satisfactory. To tackle the convergence problem related to the pressure field in the tube using rhoPimpleFoam solver, I decided to conduct a preliminary simulation without considering the heat flux.
In this regard, I successfully resolved the convergence issue by adjusting the solver in fvSolution. I switched from using PCG to GAMG, which led to the desired results.
However, when I introduced the heat flux at the wall and re-ran the simulation with the multiphaseEulerFoam, I observed that the temperature does not rise at all. So would share my complete case file to seek further insights and assistance. Maybe If necessary I'll just create a new discussion thread with a suitable title to facilitate targeted discussions.
Thank you again!

[Mytho]

Originally Posted by Yann

Mytho started rhoPimpleFoam using mpirun, but he forgot to add the -parallel option for the solver so it started n serial rhoPimpleFoam processes rather than running the solver in parallel mode.

@Mytho, the proper syntax should be something like this:

mpirun -np core-number-you-want-to-use rhoPimpleFoam -parallel

However this won't change the convergence issue, so Tobermory's comments are still on point.

Regards,
Yann

Hi Yann,
Thank you i didn't notice that i forgot the "-parallel" in my command. I appreciate it