[MMoataz]

I finished the simulation of each side of a shell and coil heat exchanger on its own and they give correct results, however, when I combine both sides together to simulate the whole system, I strangely get wrong pressure distribution in the shell side after convergence!

My questions are:
- How could the presence of the 2 domains together affect results?
- What can be done to fix this?

Summary of used settings:
- All solid and fluid bodies share topology
- Solver: Pressure based - Coupled
- Working fluid in shell: air
- Working fluid in coils: thermal oil (density 850 kg/m^3)
- Turbulence model: SST
- Both fluids have mass-flow-inlet and pressure-outlet BC
- Each fluid is initialized separately
- Default methods and controls

Note that the same mesh and same settings are used when simulating each side separately or when simulating both of them together!

[Muhammad Saad]

Hello brother I am also facing something like this.... I dont understand why my pressure results are off..... my heat transfer coefficient is okay..... on research gate one person told me that my friction factor might be wrong so I should check for reference values and wall roughness it didnt help me but might help you.... if you do find solution do give an update on this post on how you did so..

[MMoataz]

Hello Muhammad,
you will have to set the operating density to zero to fix this problem.

To do this go to boundary conditions > click operating conditions button > check on "Specify operating density" checkbox > enter a value of zero in the field

This problem happens because when you don't set the density, fluent will assume the density to be the average density. This is OK when one fluid is in the system but when 2 or more fluids of large density differences exist this assumption causes this problem.

reference
https://www.afs.enea.it/project/nept...fer-op-density

[pakk]

Originally Posted by MMoataz

Hello Muhammad,
you will have to set the operating density to zero to fix this problem.

To do this go to boundary conditions > click operating conditions button > check on "Specify operating density" checkbox > enter a value of zero in the field

This problem happens because when you don't set the density, fluent will assume the density to be the average density. This is OK when one fluid is in the system but when 2 or more fluids of large density differences exist this assumption causes this problem.

reference
https://www.afs.enea.it/project/nept...fer-op-density

You may have found the problem (I don't know), but it makes no sense that setting the reference pressure to zero could solve the problem. It could only make it worse : Fluent will then try the density associated with zero pressure (so zero density), and you will get many divide by zero errors.

Setting the reference pressure to the average pressure of your fluid pressures makes more sense. Don't forget to adjust your gauge pressures accordingly.

[Muhammad Saad]

Originally Posted by pakk

You may have found the problem (I don't know), but it makes no sense that setting the reference pressure to zero could solve the problem. It could only make it worse : Fluent will then try the density associated with zero pressure (so zero density), and you will get many divide by zero errors.

Setting the reference pressure to the average pressure of your fluid pressures makes more sense. Don't forget to adjust your gauge pressures accordingly.

Hello brother by reference pressure do you mean putting average pressure in reference values tab, and where to adjust gauge pressure( in operating conditions). I have just started cfd so I am a bit unfamiliar with fluent.... thanks for feedback for both of you.