[acro]

I tried to rotate a solid impeller in a stationary fluid domain. What's I am trying to do is that the solid impeller rotates by itself and pushes the surrounding fluid.

I set the the solid impeller as a rotating domain, and the fluid as a stationary domain. And tried various options for the interface between solid and fluid. But none of them worked.

Could anybody guide me? Thanks a lot.

[Attesz]

Hi,

I think it will not working. You have do define the fluid as a rotating domain, to set to the flow tangencial velocity component. But why do you want to do your simulation this way? Wit rotating domain option, you can get very accurate results, with transient simulation you can set "Transient Rotor Stator" Frame Change model, which "rotates" the domain...

Attesz

[acro]

Originally Posted by Attesz

Hi,

I think it will not working. You have do define the fluid as a rotating domain, to set to the flow tangencial velocity component. But why do you want to do your simulation this way? Wit rotating domain option, you can get very accurate results, with transient simulation you can set "Transient Rotor Stator" Frame Change model, which "rotates" the domain...

Attesz

Thanks for your reply.

What you suggested is: set the fluid as a rotating domain. How about the solid domain? stationary or rotating? Do I need to make some settings to the interface?

Now that CFX can set a solid as a rotating domain, I suppose this option is somehow useful. But if I set solid as rotating domain and fluid as stationary domain, it turned out that the solid rotation has no effect on the fluid flow. I guess I might miss some settings?

[stumpy]

Rotating solid domains essentially add a rotational advection term to the energy equation in the solid domain, so they are only needed when you need to account for the advection of energy due to the rotation of the solid domain (e.g. a brake disk). In your case just use a rotating fluid domain and a stationary solid domain.

[Attesz]

The solid domain is useful, when you want to take into account the heat transfer for example. Of course, you have to make it rotating. But this rotation will not rotate the flow, you have to define it separately. Otherwise, in first step, you should simulate only the flow field. Taking into account of the solid body is a refinement. The walls of the rotating body will be set rotating. If there are standing walls in the rotating body, you have to set them "Counter Rotating Walls". But I think, there is a good tutorial about it in CFX help!

Good luck,
Attesz

[acro]

Thank Attesz and stumpy. I asked questions in other forums, but never got quick answers like here. I appreciate your kind help very much.

Back to my question.

My goal is to simulate a solid impeller pushing liquid. But what you suggested is to make the liquid rotating by itself. Sounds like different from the original problem. Can this kind of simulation give me accurate flow pattern just like the stationary liquid is pushed by a rotating impeller?


By the way, I do need to do conjugate heat transfer. The impeller (actually it's not a real impeller, just some solid bodies with irregular shape) generates heat.

[Attesz]

This kind of simulation is the general method for modelling rotating things. I"ve never heard, and I've got absolutely no idea how to do that, what do you want!
If the solid body has effect to the flow, then model it, but note, that you need more cells.

Otherwise, I'm simulating now an RC quad rotor helicopter's propeller. We have measures for the trust, and the difference between CFD and measure is very small. We made the simulation before, to check the goodness of the propeller blades, and after that we measured them. Without solids. But by using rotating fluid domain, like we said.

Regards,
Attesz

[Omid]

Hi buddies
I want to simulate a simple physic environment, in which one's outlet would be another's inlet, the first's outlet flow will receive to second domain after about 20 seconds, how could I define this correlation?
Regards,
Omid.

[ghorrocks]

Periodic boundaries can do it - but not with a time delay.

[AlexRonto]

Hello to everyone,

I want to make a CHT transient analysis in CFX of an electric generator. It is actually two rotating disks and a stationary rim between them.

At the beginning, I ran an analysis with no Heat Transfer and no solid domains. I created a stationary fluid domain and I set the boundaries of the two rotors as Rotating Walls and the outer boundaries of the fluid domain as atmospheric boundaries, hence I simulated the induced by the rotation flow. The results were fine, which means that (apart from achieved convergence and physically reasonable streamlines) the mass flow that I calculated in CFX-Post at a user specified surface was very close to the mass flow that is estimated through experimental measurements (about 0.045 kg/s).

When I made a CHT analysis, I set two rotating solid domains (discs), one stationary solid domain (rim) and a stationary fluid domain. The fluid-rotors interfaces were set with a Transient Rotor frame change/mixing model. I found this setup to be the most appropriate for my case.

However, at the results of the CHT analysis the mass flow at the same user specified surface as before, is much smaller (0.013 kg/s). Is there something wrong with the rotation setup?

It seems quite strange to me that CFX calculates the flow "as expected" at first, but it cannot calculate it when Heat Transfer comes in.

[ghorrocks]

I cannot say anything too specific as your description is very vague.

But some comments: Are you using a compressible gas? Heat transfer can affect the mass flow in that case.

Have you done a sensitivity check of the key parameters of your model? If not then you are comparing a random number to another random number and the comparison is meaningless.

[AlexRonto]

Originally Posted by ghorrocks

I cannot say anything too specific as your description is very vague.

But some comments: Are you using a compressible gas? Heat transfer can affect the mass flow in that case.

Have you done a sensitivity check of the key parameters of your model? If not then you are comparing a random number to another random number and the comparison is meaningless.

Thank you for your answer Glenn.

The gas I use is air at 25°C and according to the results the density is constant throughout the domain. Besides, no buoyancy effects are included. So would it be possible for the heat transfer to affect the mass flow?

I did a sensitivity study referring to the mesh density, the domain size and the timesteps for the no-heat-transfer analysis. The calculated mass flow does not change very much (from 0.038 to 0.045 kg/s).

To be more specific, I attach an image of half the machine (one rotor and half of the stator). The mass flow I calculate is the one that passes trough the air-gaps of the rotor. I define a user surface as it looks at the second image (grey area).

My question is this: Since the only thing that I changed from the first simulation to the CHT one is the mesh and the "way of setting the rotation" (rotating domains instead of rotating walls), I suppose that a different solution arises from the different "way of setting the rotation". Could it be true? If yes, is it computationally explained somehow? Could it be a mesh problem?

[ghorrocks]

So would it be possible for the heat transfer to affect the mass flow?

Yes, but if you are using a constant density fluid then your model will not have these effects.

Your comment about rotating domain versus rotating wall sounds more likely to be the reason. Can you show an image of both simulations and what boundary conditions you applied?

[AlexRonto]

I attache images of each domain that I use in the CHT analysis. In the no-heat-transfer analysis (is there a more appropriate name for this analysis??) I use only the fluid domain. The BC's are:

No heat transfer analysis
Fluid Domain
Domain motion: Stationary
Turbulence model: Shear Stress Transport

a) Outer boundaries=Openings
Mass and Momentum: Entrainment with Pstatic=0Pa (relative pressure)
Turbulence: Zero gradient

b) "Interface" with rotors boundaries (=the surfaces of the rotors that come in touch with the fluid)
No slip walls
Rotating walls: ω=17rad/sec

c) "Interface" with stator boundaries
No slip wall

CHT
1) Fluid Domain
Domain motion: Stationary
Heat Transfer: Total Energy
Turbulence model: Shear Stress Transport

a) Outer boundaries=Openings
Mass and Momentum: Entrainment with Pstatic=0Pa (relative pressure)
Turbulence: Zero gradient
Heat Transfer: Opening temperature=25°C

b) Fluid-Rotors Interface:No slip walls
Rotating walls with 17 rad /sec

c) Fluid-Stator Interface:No slip walls
Stationary walls

2) Rotors Domains (2 domains, same bc's)
Domain motion: Rotating with 17 rad/sec
Heat Transfer: Thermal energy

3) Stator Domain
Domain motion: Stationary
Heat transfer Thermal energy

HeatSource Subdomain (the same volume as the domain one, which means the stator volume. In other words, I set the stator volume to be the heat source)
Source: 2000W

4) Interfaces
Fluid-Rotors Interface
Frame Change/Mixing model: Transient Rotor Stator

Fluid-Stator Interface
Frame Change/Mixing model: None


I tried to include what I think is the most important characteristics of my simulations. Maybe some details are missing ..

[ghorrocks]

The rotor has the cut out sections in it, doesn't it? So those pieces won't move when you do a steady state, stationary simulation. When you apply a wall velocity it means the wall has a tangential velocity applied but the mesh does not move. This is very different to the true rotating case.

[AlexRonto]

Originally Posted by ghorrocks

The rotor has the cut out sections in it, doesn't it? So those pieces won't move when you do a steady state, stationary simulation. When you apply a wall velocity it means the wall has a tangential velocity applied but the mesh does not move. This is very different to the true rotating case.

That's why I ran a transient analysis (in both cases) and I also allowed a mesh motion (nevertheless,at the results and at the output file, the mesh displacements are zero at any time step).

So what I understand is that, in order to capture the rotating movement of the cut out sections, I have to allow the cut outs to change position at the mesh grid during the simulation and at the same time, at every new position the cut outs' nodes should have a constant tangential velocity.

Is my interpretation correct? And if yes, is the transient analysis and mesh displacement settings the appropriate ones?