[ssbear]

Hi everyone,

I'm new to CFD and I'm now trying to make a water intake model. In my model, the inlet is set to be 3 m/s (normal speed) and the outlet is also set to be 3m/s (normal speed). For the gravity effect, I used two ways to simulate it:

1. free surface model as shown in tutorial 7
2. single-phase model with sub-domain to simulate the gravity (general momentum source)

Now the resutls of both ways are quite different and I'm just wondering which one makes more sense ?

Thanks in advance for any advice!!

[mvoss]

hi,
do you want to compare multiphase vs. singlephase?

Btw. you can set the gravity without any subdomain by just setting the vector properly (look up gravity in the help).

neewbie

[ghorrocks]

You model gravity using the gravity option. Forget about source terms, it is already in there, you just need to activate it.

Your boundary conditions are probably poorly defined as pressure is not set anywhere. You need to set a pressure somewhere.

[ssbear]

Originally Posted by ghorrocks

You model gravity using the gravity option. Forget about source terms, it is already in there, you just need to activate it.

Your boundary conditions are probably poorly defined as pressure is not set anywhere. You need to set a pressure somewhere.

Originally Posted by neewbie

hi,
do you want to compare multiphase vs. singlephase?

Btw. you can set the gravity without any subdomain by just setting the vector properly (look up gravity in the help).

neewbie

neewbie and ghorrocks,

Thanks for your advice. I'm not comapring multi-phase vs single-phase. It's just I don't know how to set the gravity effect properly. As you know, for single-phase, in the domain setting we can only find Boussinesq Model for buoyancy, which is not useful in my case. And I don't know other way other than using sub-domain to define gravity in single-phase model (which I found in one of ghorrocks's old thread).

I've been stuk here for a while and the help in CFX doesnt explain too much either. It will be appreciated if you guys can show me how to do it in a little more detail.

Thanks!!

[ghorrocks]

For a single phase what would gravity affect? I think you will find gravity has no effect when you simplify it to single phase.

Gravity affects a multiphase (free surface) simulation by pulling the heavy fluid to the bottom. You definitely need gravity in this case. Activate it simply by setting the gravity vector. An example is the flow over a bump tutorial example.

[ssbear]

Originally Posted by ghorrocks

For a single phase what would gravity affect? I think you will find gravity has no effect when you simplify it to single phase.

Gravity affects a multiphase (free surface) simulation by pulling the heavy fluid to the bottom. You definitely need gravity in this case. Activate it simply by setting the gravity vector. An example is the flow over a bump tutorial example.

Thanks for your reply, ghorrocks. My question and main purpose right now is find the easiest way to simulate the flow in my case. Apparently to me single-phase flow is simpler than free surface flow. Another reason I don't prefer free surface model is that it can't simulate the particle tracking which I will be doing later on.

My problem for the single-phase model is if I don't set the gravity effect , the flow pattern doesn't make sense to me (please see the attached figure). So I was looking for a way to add gravity in single-phase model in this forum and the only way I found is to use the sub-domain.

It would be beautiful if there is an easier way to set the gravity effect in the single phase model. Please let me know.

BTW, by looking at the results from both methods I posted earlier, which one makes more sense to you?

Thanks very much for your advice and I'm looking forward to your reply!!

[ghorrocks]

What are you trying to model? You need to tailor the model to what you are trying to achieve. What is the purpose of doing your simulation?

[ssbear]

Originally Posted by ghorrocks

What are you trying to model? You need to tailor the model to what you are trying to achieve. What is the purpose of doing your simulation?

The main purpose of this practise is to simulate the flow in the intake and sediment movement.

I'm now trying to get the correct model, so later on I can change the intake geometry to optimize the flow. I'm a structural engineer and am new to CFD, so sometimes I might have some stupid question...

[ghorrocks]

Does the free surface move? Is it flat?

[ssbear]

Originally Posted by ghorrocks

Does the free surface move? Is it flat?

No. There is a little curve at where the geometry trasition. Please see the attached pic, the green line at top is the water surface.

[ghorrocks]

So it is pretty flat. Is the little wobbles in the surface important? If you are modelling sedimentation then I do not think so. In this case you can run this simulation as single phase with a pressure boundary replacing the free surface. Single phase models are much easier and quicker so if this approximation is OK for you it will make things much easier.

[ssbear]

Originally Posted by ghorrocks

So it is pretty flat. Is the little wobbles in the surface important? If you are modelling sedimentation then I do not think so. In this case you can run this simulation as single phase with a pressure boundary replacing the free surface. Single phase models are much easier and quicker so if this approximation is OK for you it will make things much easier.

Thanks, ghorrocks~~
Will let you know when I finish my sediment model.

[ghorrocks]

Be aware that CFX has limited capabilities in sediment modelling. The lagrangian particle tracking works fine, but it does not have models of sedimentation, picking up of sediment or good packing models. You may be able to develop these models yourself (that is not a task for a beginner!) or you could couple CFX with a discrete element model (DEM) such as EDEM to do the bits CFX cannot.

But I do not know whether this is important to you or not as you have not described your model in sufficient detail. The stuff built into CFX may be fine for you.

[ssbear]

Originally Posted by ghorrocks

Be aware that CFX has limited capabilities in sediment modelling. The lagrangian particle tracking works fine, but it does not have models of sedimentation, picking up of sediment or good packing models. You may be able to develop these models yourself (that is not a task for a beginner!) or you could couple CFX with a discrete element model (DEM) such as EDEM to do the bits CFX cannot.

But I do not know whether this is important to you or not as you have not described your model in sufficient detail. The stuff built into CFX may be fine for you.

Thanks, ghorrocks. The feature in CFX is good enough for me for now.

I'm now trying to make the particle tracking model. My BC would be:

Inlet: normal speed = 2.5m/s (same speed for particle)
Outlet: static press = P, where P is the water pressure varies with the depth
Default domain: rough wall with 0.4mm roughness


Does that make sense to you?

Looking forward to your suggestions. Thanks very much!

[ghorrocks]

If you are modelling this single phase (and from your description so far I think you can) then do not model gravity and do not use a static pressure head on the outlet. Just a single pressure value.

Other than that your model should work. I have no idea if it is appropriate, however - that is for you to decide.

[ssbear]

Originally Posted by ghorrocks

If you are modelling this single phase (and from your description so far I think you can) then do not model gravity and do not use a static pressure head on the outlet. Just a single pressure value.

Other than that your model should work. I have no idea if it is appropriate, however - that is for you to decide.

Thanks, ghorrocks.

Yes, I'm modeling the signle phase.

In my project, the water in this intake structure has a free-surface. The outlet is the submerged penstock that is connecting to the turbine generate which allows a maximum flow of 29 m3/s. Assuming that maximum flow, I set my inlet BC as normal speed = 2.5 m/s, but I'm not sure which pressure value I should use for my outlet BC. Should I just set it to 0 Pa?

Don't know if there's enough information for the problem, but still looking forward to your precious advice.

Thanks~~~

[ghorrocks]

Do not make boundary conditions up. If you know the outlet flow which connects to a known turbine flow rate, then make that the boundary - so use 29 m3/s on the outlet. Then put a pressure boundary at 0Pa on the inlet and it should work fine.

[ssbear]

Originally Posted by ghorrocks

Do not make boundary conditions up. If you know the outlet flow which connects to a known turbine flow rate, then make that the boundary - so use 29 m3/s on the outlet. Then put a pressure boundary at 0Pa on the inlet and it should work fine.

Thanks, ghorrocks!

Will try it and let you know the result.

[ssbear]

Originally Posted by ghorrocks

Do not make boundary conditions up. If you know the outlet flow which connects to a known turbine flow rate, then make that the boundary - so use 29 m3/s on the outlet. Then put a pressure boundary at 0Pa on the inlet and it should work fine.

ghorrocks,

I tried the particle model and there is something that doesn't look right. The particles in the water drop to the buttom of the domain and then climb up the slope... Is that because I didn't set the gravity correct? The particle here is sand (2300 kg/m3) at the diameter of around 1-3mm.

From the flow diagram, it shows that flow is going uphill on the slope, which doesn't make sense to me either...

Sorry for so many questions and thanks for your help.

[ghorrocks]

I do not think you looked at your results very hard.....

The particles are simply falling out of the flow due to their weight and hitting the bottom wall. You have modelled a big separation which results in a reverse flow up the slope. This reverse flow is pulling the sand up the slope.