[hutudx]

I ran some test cases on a simple mixing tank as shown in the attached geometry file. Because there is no baffles and other angular-dependent internal components (such as dip tubes, etc.), I think that SRF (single reference frame with rotation), MRF (multiple reference frame -- 1 static domain and a rotating domain containing impeller) and sliding mesh are all perfectly suitable for this problem. But I got quite different torque values from 3 different methods. In addition, even just for MRF method, the torque values are different if different size rotating domain are used (the difference is not small -- could be 30% different).

I am wondering if anybody have similar experience and how to explain it. I searched online and found very little information on this, especially with Fluent, which is surprise to me.

[vinerm]

You can use MRF or moving mesh, however, SRF is not valid in this case since you have one rotating domain and one stationary domain. Moving mesh will give fluctuating torque, however, average should be closer to MRF. It can be very different if there are integral size eddies crossing the interface.

[hutudx]

Thank you for your reply.

Actually, when using SRF, I only have one domain. I did not attach a separate picture for it. Sorry for confusion.

[vinerm]

That makes sense

[hutudx]

Because there is no baffles and other angular-dependent components, I think that even sliding mesh should yield a constant value (imagine an observer rotating with the impeller, what he sees is a steady state problem). But actually, I did see fluctuating in torque value with coarse mesh, oscillation eventually faded away with finer mesh. The problem is that the converged value is different from MRF and SRF values (they are different to each other themselves)

[vinerm]

Even without any blades or baffles, there are turbulent eddies that would cause interference at the interface. However, as I mentioned earlier, the average should be close to MRF. If that is not the case, then you need to dig a little deeper. A few thing to check

1. Overall mesh and particularly mesh at the interface
2. Rotation speed. If it is low, then even MRF should be run in transient. Low implies anything lower than 3 Hz. General recommendation is 5 Hz.
3. Convergence of the cases

[hutudx]

Thanks again.

The case I simulated is 180rpm. And the torque history are shown in the attached file. It seems to me that they converged well.

[vinerm]

Were these cases run in single precision or double precision? Since the values themselves are rather small, these have to be run in double precision. Though the actual basis for dp is if gradients are very low in the domain yet for small values of the field variables, dp improves the results.

Furthermore, from the monitor view points these look converged. What about the residual values? Residuals are not always very important but for cases with small values, these become important. If residuals themselves are of the same order as those of field values, then solution is not converged. That was my primary reason for asking about convergence. In Fluent's language, this is called convergence depth. If residuals are still high, you can use higher order schemes to improve those. Coupled solver improve the results for rotating machines.

[hutudx]

Very good discussion. Actually, I tried many things (dp vs. sp, higher order vs. lower order, finer mesh vs. coarse mesh at interface, boundary layer mesh at interface, etc.) Interestingly, what I found so far is that the results from higher order and lower order is quite different themselves, but did not solve the difference between MRF and sliding mesh methods. Finer mesh at interface definitely help convergence for sliding mesh method but did not reconcile difference between methods either. Boundary layer mesh at interface seems to make convergence worse. I tried dp once and seems making little difference, but not very sure about it yet.

[vinerm]

As far as order is concerned, if converged, higher order is better than lower. So, you can trust higher one. For the mesh, putting boundary layer at the interface could cause disturbance if the finer eddies begin to show up. That would require smaller to stabilize.

For industrial use, my recommendation is to always use dp. I have never run a simulation in sp.

[hutudx]

vinerm, thank you for discussion. A related question: do you think MRF results will depend on the rotating domain size. Somebody say yes. But if it is the case, how do we know what the right size is?

[vinerm]

Yes, size does matter. The size should be as close to the rotating body as possible. If diameter of actual rotating impeller is 100 mm then diameter of MRF should be as close to 100 mm as possible. The reason for this is simple. In case of MRF, forces are added as momentum source throughout the domain that is rotating. Now, the distribution is a radial function but not a function of circumference, which is a reality in a real impeller. Therefore, moving mesh is better than MRF and size of MRF should be as close to impeller size as possible

[hutudx]

Is this right? If this is the case, then the SRF method won't be valid. Did I misunderstand something here?

[vinerm]

SRF is valid if you considered only the small domain around the rotor. If you considered whole of the domain as SRF, then that would lead to very wrong results.

[hutudx]

Hmmm.... I need to think about it. I think an observer rotating with impeller should be able to solve the problem correctly in his configuration.

[vinerm]

The issue is not with the reference frame. The challenge comes from the reason for the flow. Since whole of the domain is looked at from the observer who is rotating with the domain, if there is no source, there is no motion. The fluid body will rotate like a solid body from an initial reference view point. Due to the motion of the rotor, centrifugal and Coriolis forces are to be added to each cell. In reality, these should only be added to the cells adjacent to the boundaries of the rotating solid body. Since that is not possible with either SRF, MRF, or moving mesh, force is added to entire domain but source value is non-uniform.

[damon707]

Hello all,

Continuing the same discussion, I want to simulate a wind turbine rotor (blades and hub only) with SRFSimpleFoam. Currently I have a cylindrical computational domain as shown in the picture.The radius of the rotor is R=1.19m and the radius of the cylindrical domain is 5R.
I cant get a physical solution. I get a converged solution but the result is quite unphysical, there is not even a wake formed behind the rotor. Is this wrong result due to the size of the cylindrical computational domain? Where can I find info on how exactly the size of the domain affects the accuracy of an SRF simulation?

Best,
George