[minzhang]

Ansys/Fluent/Multiphase

Hello All,

I am using the Eulerian-Eulerian two-fluid model (in Ansys Fluent) to simulate the turbulent solid-liquid two-phase flow in a horizontal pipe.
This is the reference paper I am trying to reproduce:
Eulerian-Eulerian Simulation of Particle-Liquid Slurry Flow in Horizontal Pipe
Titus Ntow Ofei and Aidil Yunus Ismail

Currently, I am quite sure about my physical model settings. But my simulation is not converging and please see the attachment.
I think the settings that I can play with are Solution Controls, Method Controls, and mesh.

In addition, except for playing with the current model, I am also thinking to first simulate a laminar flow and then add the turbulence model.

Your valuable comments would be greatly appreciated!

[minzhang]

For the current model:
1. I reduced the inlet velocity to have a smaller Reynolds number (but it is still turbulent flow), it didn't converge.
2. I used a very small inlet velocity to have a laminar flow, it didn't converge.

Then, I thought it might be due to the mesh quality.

3. I even established a new model on another reference paper. It seems for me it won't converge (please see the attachment). In this case, I think the mesh should be fine.
This is the reference:
Sand Transport and Deposition Behaviour in Subsea Pipelines for Flow Assurance. Yan Yang, Haoping Peng and Chuang Wen.

4. In addition, I saw some Console outputs before crashing:
Reversed flow on 2 faces of pressure-outlet 5.
Stabilizing epsilon to enhance linear solver robustness.
Stabilizing epsilon using GMRES to enhance linear solver robustness.
turbulent viscosity limited to viscosity ratio of 1.000000e+05 in 465776 cells

Currently, I am thinking I might need to degrade my case further to ONLY simulate turbulent fluid flow first, then add the solid phase.

Your valuable comments would be very appreciated!

[minzhang]

Please see the attachments of both the Graphics and Console output.

Your comments would be very appreciated!

[vinerm]

The image you showed in the second last post shows convergence, however, the latest one does seem to have some issues. Laminar cases are more difficult to converge than the turbulent ones since the momentum does not diffuse and cause numerical instabilities that require higher order models for resolution. What you call non-convergence is the expected behavior for a transient case. The simulation is supposed to converge in each time-step, hence, the residuals appear to oscillate. In reality, these are convergence plots for each time-step joined together. Hence, they appear as not converging.

[minzhang]

Thank you so much for your reply!

How about the Console outputs? It seems that the epsilon equation blows up and also the turbulent viscosity calculation has some issues?

Originally Posted by vinerm

The image you showed in the second last post shows convergence, however, the latest one does seem to have some issues. Laminar cases are more difficult to converge than the turbulent ones since the momentum does not diffuse and cause numerical instabilities that require higher order models for resolution. What you call non-convergence is the expected behavior for a transient case. The simulation is supposed to converge in each time-step, hence, the residuals appear to oscillate. In reality, these are convergence plots for each time-step joined together. Hence, they appear as not converging.

[vinerm]

As per your last post with the images, yes, the solver is facing difficulty. However, this could be due to anything, starting from a bad mesh all the way down to numerical schemes. You have to ensure that the mesh is good. All material properties, boundary conditions, phase interactions, and operating conditions are good. Then check numerical setup, such as, discretization schemes, pressure-velocity coupling, and URF, etc. You may also try a smaller time-step. If the simulation requires more than 30-40 iterations per time-step for convergence, then your time-step is large for the setup.

[minzhang]

More info:

For the first reference paper:

The case I am trying to reproduce is: particle diameter = 270microns, particle volume fraction = 0.1.

The paper was using CFX and I am using Fluent.

The settings I am using are consistent with the settings mentioned in the paper. The settings that the paper did not mention and I think they might influence my simulation results are listed below.

In addition, there is a difference between their geometry and mine. In their paper, L=44D, and cell no. = 801,848. Since I am using the student free version and I have the limit of 512,000 cell number. So in my case, L=25D and my cell no. = 508,600. My mesh might be different from theirs but I think my mesh resolution should be fine compared with theirs. Please see the attached screenshot of my mesh.

My Scaled Residuals plot is also attached.

Your valuable comments would be very very appreciated!!

Settings were not mentioned in the paper:

1. Materials - Fluid - solid: what is the viscosity value? (1e-6 kg/(m.s))

2. Multiphase Model - Phases - Secondary Phase - Granular Conductivity: syamlal-obrien

3. Multiphase Model - Phases - Secondary Phase - Frictional Viscosity: shaeffer

4. Multiphase Model - Phases - Secondary Phase - Frictional Pressure: Johnson-et-al

5. Multiphase Model - Phases - Secondary Phase - Radial Distribution: lun-et-al

6. Multiphase Model - Phase Interaction - Forces - Drag Coefficient: gidaspow

7. Viscous Model - Turbulence Multiphase Model: Per Phase

8. Velocity Inlet - Turbulence - Turbulent Intensity: 3

Velocity Inlet - Turbulence - Hydraulic Diameter: 0.0072

Velocity Inlet - Granular Temperature: 0.007272

9. Pressure Outlet - Backflow Turbulent Intensity: 0

Pressure Outlet - Backflow Turbulent Viscosity Ratio: 0

Pressure Outlet - Backflow Granular Temperature: 0

Pressure Outlet - Backflow Volume Fraction: 0

10: Wall - Granular Conditions: Johnson-Jackson

Wall - Granular Properties - Restitution Coefficient: 0.2

[vinerm]

If volume fraction is only 0.1, you should not use Granular model. I suppose you have got the number wrong because 0.1 particle volume fraction does not imply a slurry. So, I'd suggest you verify this number. And if it is really less than 10%, use DPM; that's more accurate.

[minzhang]

Hello vinerm,

The particle volume fraction is 10%-45%. 0.1 means 10%, is that right?

Originally Posted by vinerm

If volume fraction is only 0.1, you should not use Granular model. I suppose you have got the number wrong because 0.1 particle volume fraction does not imply a slurry. So, I'd suggest you verify this number. And if it is really less than 10%, use DPM; that's more accurate.

[vinerm]

Yes, then granular makes sense. Instead of using per phase turbulence, use mixture. Do not set flow reversal parameters to 0. If there is flow reversal in the beginning, it will cause trouble. Only pressure should be set to 0. For others, use some positive values.

[minzhang]

I am wondering how to decide the backflow parameters? What would these non-zero backflow parameters do?

Thanks!

[vinerm]

If there is no flow reversal at the outlet for you case, then these values are not used. However, if there is a flow reversal at the outlet, then the outlet begins to behave like inlet. And for inlet, Fluent requires inlet conditions. So, you can use conditions similar to you inlet.

[minzhang]

If the calculated velocity at one outlet cell is -1m/s, then the outlet boundary condition will adjust this value to be backflow parameter, for example, +5m/s. Is that correct?

[vinerm]

The velocity for the backflow does not depend on the velocity of the outgoing flow. It depends on the pressure in the cell adjacent to the outlet. If the pressure reduces below the pressure at the outlet, then the flow starts to reverse. Flow rate or velocity will depend upon the difference in the pressures at the outlet and first cell adjacent to the outlet.

[minzhang]

If the pressure at the first cell adjacent to the outlet reduces below the pressure at the outlet, then the flow starts to reverse.

Then, what will happen if I have a backflow condition which is the same as the inlet condition?

Thanks!

[minzhang]

I made these changes, but it still could not converge.

Originally Posted by vinerm

Yes, then granular makes sense. Instead of using per phase turbulence, use mixture. Do not set flow reversal parameters to 0. If there is flow reversal in the beginning, it will cause trouble. Only pressure should be set to 0. For others, use some positive values.

[vinerm]

When I mentioned that you can maintain similar conditions as inlet, I did not mean the pressure as well. Until unless the pressure is lower than the inlet, flow cannot pass though. Pressure at the inlet should be left at 0. For turbulence quantities, you can use similar values. Volume fraction of secondary phase can be left as 0 as well.

[minzhang]

I gave the "Supersonic/Initial Gauge Pressure" = 0 for my Velocity Inlet. I think this is only an initial pressure value for the velocity inlet. The solver will calculate the pressure at the inlet, which will be higher than 0.

For my Pressure Outlet, the Gauge Pressure = 0.

Originally Posted by vinerm

When I mentioned that you can maintain similar conditions as inlet, I did not mean the pressure as well. Until unless the pressure is lower than the inlet, flow cannot pass though. Pressure at the inlet should be left at 0. For turbulence quantities, you can use similar values. Volume fraction of secondary phase can be left as 0 as well.

[vinerm]

Yes, that's correct.

[minzhang]

Since I still could not have a converged result, the only option I have now is to have a refined mesh. Is that right?

In addition, I am wondering what are the possible reasons that I could not reproduce that reference paper?

Thanks!