[Rubblevg]

Hi,

I am currently having trouble with implementing gravity in a 2D flow model. My model basically consists of a large square with a (low velocity) inlet and a (pressure) outlet above each other on the same wall.

The solution converges fine until I try to implement gravity. As soon as I turn gravity on (in any direction) nothing changes to the static pressure profile, unless I also introduce a reference density rho_0 of zero. This makes sense because the static pressure p_s' is defined in Ansys as:
p_s' = p_s - rho_0*g*y
From this it follows that in order to be able to use the real static pressure I need to have a rho_0 equal to zero. Several sources I found also recommended this value for rho_0 for flows where gravity may play a large role in the fluid movement.

However, when I set rho_0 to zero I start having two problems which I think are linked together. First of all, the solution starts having a lot of convergence problems. Besides that, significant, unrealistic backflow can be distinguished at the pressure outlet. There seems to be some sort of recirculation through the outlet, but if I place a pipe between the outlet and the wall, the recirculation remains at the outlet instead of the zone where the pipe connects to the wall.

Does anyone know what the problem is with my setup and how to fix it? I think something is wrong with the boundary conditions of my pressure outlet, but I haven't found a way to solve it. I tried to refine the mesh, apply different integration schemes, change relaxation factors and move the outlet more downstream by adding a pipe between it and the wall

[KevinZ09]

I'm assuming your fluid flows counter-gravity?

Either way, when you say "reference density", do you really mean the reference density as specified in the Reference Values panel, or do you mean the Specified Operating Density? The latter is the rho_0 appearing in the p_s' = p_s - rho_0*g*x equation, while the former is used for post-processing. Since it affects your results, I assume it's the latter.


You're correct in stating that Fleunt removes the hydrostatic head in it's calculations, and if you want to actually resolve for this hydrostatic pressure, you need to set rho_0 = 0 and specify a reference density equal to your fluid density. However, as you experienced, this could lead to convergence problems because these body forces are quite large, potentially leading to large numerical errors. So it probably will take longer for your simulation to converge and for the backflow to disappear.

But what is it precisely you're trying to model? I normally don't specify any operating density, and thus Fluent uses a volume average, but that's also because I generally am not really interested in the hydrostatic pressure (which I could simply add if I were interested in it). So, two questions:
- What are you trying to model?
- Why would you want to resolve the hydrostatic pressure explicitely?

[Rubblevg]

Hi Kevin,

Thank you for your response. The fluid flows indeed counter-gravity and you are also right about that I actually meant the specific operating density.

What I am trying to model is a bioreactor which basically consists of a container filled with liquid and small particles on which living cells can grow. The inlet and outlet that I mentioned are used to add nutrients to the system and remove waste products. Furthermore, the reactor keeps the particles in suspension by turning 180 degrees every time interval t. Right now I am trying to model the bioreactor with only the fluid phase present (without mixing) and I want to know the influence of gravity on the circulation flow. If gravity has a neglicible influence on the single-phase flow, I think I can leave the operating density unspecified when I add the particle phase to the system, because gravity only plays a role in buoyant effects. Is this reasoning correct?

If I understood correctly, Fluent neglects gravity when the operating density is left unspecified. This is because p_s' = p_s - rho_0*g*x, which is the same as p_s' = p_s - rho*g*x, since the flow is incompressible and Fluent takes the operating density to be the volume averaged density (so rho_0 = rho). Therefore, modelling the hydrostatic pressure explicitly is the only way of really introducing gravity to the 1-phase system right?

I hope this answers your questions and I would like to hear your view on my method!

[KevinZ09]

I agree with you that when you leave the operating density unspecified, and that your case has a constant density, that buoyancy effects are not present. Also, yes, setting the operating density to zero will allow you to explicitely resolve the hydrostatic pressure. I'm just curious as to what you're so interested in the hydrostatic pressure in a single-phase flow?

As for what the operating density should be in a multi-phase flow, I'd advice to use the density of the lightest phase. This way you remove the hydrostatic pressure from that phase and improve the accuracy of the round-off errors. But you can experiment with it to see what works best for your particular case.

[Rubblevg]

Hi Kevin,

It's not that I am necessarily interested in the hydrostatic pressure itself. I only want to find out if gravity has any influence on the 1-phase flow, besides buoyancy effects. Because it seems to me that gravity is completely neglected for an incompressible 1-phase flow if the operating density remains unspecified, I want to run simulations with an operating density of zero and thus explicitly solve hydrostatic pressure. Is this reasoning valid? Or is gravity only removed from the formulation of the hydrostatic pressure and not from the rest of the calculation if I leave the operating density unspecified?

Thanks for your advice on gravity in a multi-phase flow. I will keep that in mind.

[KevinZ09]

I'm assuming you mean an incompressible material and not an incompressible 1-phase flow? Because for an incompressible flow, the density doesn't have to be constant. For an incompressible material (constant density), I'd agree with you that (unless you use the Boussinesq approach) gravity is fully eliminated from the calculations and its value has no effect on the results. But perform some small tests and you'll get a definite answer.

[Rubblevg]

I already found out that the flow doesn't change if the density is constant (so incompressible material indeed), which makes sense because gravity is indeed eliminated for an unspecified operating density. However, does this also hold if the hydrostatic pressure is solved explicitly (so operating density = 0)? A change in hydrostatic pressure can also cause a change in dynamic pressure and thus the flow velocities right?

I agree with you that testing this would give me an answer, but that's my main problem: I cannot run tests for operating density = 0 because of the severe backflow and convergence problems. Do you have any suggestions to solve these issues?

[KevinZ09]

Originally Posted by Rubblevg

However, does this also hold if the hydrostatic pressure is solved explicitly (so operating density = 0)?

Yes, it should. It's not like Fluent is necessarily changing the equations, it just rewrites the body-force term into (rho - rho_0)*g by redefining the static pressure to p_s' = p_s -rho_0*g*x. So it just makes the terms much smaller to reduce numerical errors.

Originally Posted by Rubblevg

I agree with you that testing this would give me an answer, but that's my main problem: I cannot run tests for operating density = 0 because of the severe backflow and convergence problems. Do you have any suggestions to solve these issues?

That's exactly why Fluent changes the equations somewhat. But doesn't it converge at all or really slowly? I've had backflow in similar situations before, but it slowly dissappeared after continuing with the simulation. What settings are you using? And what fluid?

[Rubblevg]

Hi Kevin,

Sorry for my late response. Your answer helped me a lot, the concept of operating density is now much clearer to me. This means that I won't necessarily have to specify the operating density to solve my problem.

When I do specify the operating density however, my solution indeed doesn't converge at all usually. Only for a few solution methods and URF's it converges (although very slowly) and even then I have backflow in the end.

As fluid I am using water (rho = 998.2) and I use a velocity inlet of 0.001 m/s with two pressure outlets under it. I use the pressure-based solver with SIMPLE or PISO scheme and for the pressure discretization I use body force weighted. Furthermore, for the momentum discretization I use either second order or power law (apparently, power law works very well for the convergence).

For URF's I mostly try to use a low value for momentum (about 0.3) and I also slightly decrease body forces (~0.8). I leave pressure and density untouched (0.3 and 1 respectively).

Do you have any suggestions for improving these settings?

[KevinZ09]

It'll be quite problematic I guess for your case, due to the very low velocity. But some things you could try:

- Use an outflow boundary instead of a pressure outlet.
- Refine your mesh near the outlet. Make sure your mesh is fine enough, and perhaps even use long thin cells. This has been found to reduce the backflow somewhat.
- If possible, move the outlet boundary further downstream.
- You can also always play with your velocity. You may have a smaller velocity in your real case, but larger velocities could give you some indication already.
- Perhaps try first-order discretization.

These are some of the things I'd try first.

[Rubblevg]

Except for the long thin cells at the outlet, I already tried all options you suggest. How can I create these long thin cells? I cannot find it in the Ansys meshing.

Is there perhaps a way of decreasing the pressure at the outlet? In the real case there is actually a weak suction pump placed after the outlet, but I haven't found a way of modelling this. I tried decreasing the gauge pressure at the pressure outlet. However it seems the pressure over the entire domain decreases with this gauge pressure, meaning that there is still effectively no lower pressure at the outlet.

[KevinZ09]

I never use ANSYS meshing to be honest, but can't you specify like grid size or something like this? I know it's possible in Gambit.

As for the extra pressure drop at the outlet, you can create a pressure jump or porous medium zone, depending on what you're trying to model exactly.

Perhaps show your geometry, it might give me a better idea of what you could do to resolve your current issues.

[Rubblevg]

In Ansys meshing the grid size indeed can be specified. That's what I already did when refining the mesh. However, I am not sure about creating the long thin cells you mentioned.

How can I create this pressure jump at the outlet you mentioned? I know about the porous medium condition, but it doesn't seem to match the suction pump that's actually there in reality. What do you think?

My geometry is given in the attachment. Geometry 1 gives the 'real' geometry with the inlet given by the blue area and the outlet(s) given by the red area. I know that the outlet and inlet are quite close to each other, so I also tried to move the outlet boundary more downstream (see Geometry 2). This doesn't change much however. What do you think would be the solution?

[KevinZ09]

Sorry for the late reply. It has been a bit hectic at work of late.

To create this pressure jump, you could either use Porous Jump Boundary Condition or perhaps even an Exhaust Fan, which allows you to prescribe a pressure jump as well.

I do wonder, in your model, is gravity pointing downward or from left to right?

[Rubblevg]

No problem Kevin, you can take your time responding!

I'll try out the exhaust fan, thanks. How can I implement the porous jump condition? I read about it online, but cannot seem to find it in Fluent under boundary conditions. Is it a special type of interface? I only got an educational version of Fluent, maybe that's the reason I cannot find it under boundary conditions. Perhaps porous jump condition is only available in the research version Fluent.

The gravity in my model is indeed from left to right (so positive x-direction). Sorry, I forgot to indicate that in my geometry.

I also have another, not entirely related, question for which I hope you know an answer. For the granular two-phase flow in my geometry, I need to create a boundary condition that only allows the fluid phase to flow out (in reality there are filters in front of the outlet). Do you know any method in Fluent to do this?
I tried using the porous medium condition, but this only creates additional resistance rather than completely stopping the granular phase. Also I tried fixing the velocity of the granular phase at zero around the outlet by creating a seperate body there and using fix velocity at 0 in Cell zone conditions->body->phase 2->fixed values. However, unphysical and unrealistic effects arise around the interface between this zero-velocity area and the nonfixed-velocity area. It may be possible to use UDF's to constrain the granular phase to the domain, but so far I haven't found any Define_macro that could do this.