Hi! I'm a PhD student at TU-Darmstadt-Germany, and my problem is:

I'm modelling a water pump (nq12) in turbine operation in Fluent (3D) using the moving reference frames model, steady flow. I think the rotor-volute interaction isn´t to big (in the tongue it is) so I hope the integral values are good. The stagnation pressure at the impeller inlet seems to live its own life. By low volume flows (part load), p stag at impeller inlet is higher than at the spiral casing inlet, and for high flows (over load), it is much lower (which agree with the experimental mesurments) , giving an efficiency for the spiral casing at about 86%.

Ideas on why this happens would be enormously appresiated.

I´m very interested in discussing the best model for solving turbomachinery (rotor-volute interaction) in 3D. I modeled a pump without impeller channels with 712.000 hexahedral cells, and the results seems to be good. Now I want to model it with the channels and study the moments relations with the diferents clearance seals and after that, study the pump with guide vane.

Alberto Tamm Tamm@tfa.maschinenbau.tu-darmstadt.de

(1). What is your definition of "The stagnation pressure"? (2). What is your definition of "p stag at the impeller inlet"? , "p stag at the spiral casing inlet" (3). In the moving reference frame, how do you define the static presure, velocity, and the stagnation pressure?

Hello John,

Sorry for my english,

P stag = Total pressure

P tot = P stat + c^2/2g (where c the absolute velocity is)

The problem is that for part load operating condition P tot at the impeller inlet is bigger than at the turbine inlet, but for the nominal condition Delta P tot is positive and represent the friccion in the volute.

(1). You can take a look at the flow field around the impeller inlet or blade leading edge area. (2). The velocity vector field should tell you something about what's going on there.

I suggest that you run a few simulations on the impeller, without volute, with different volume flows. Then you will get an idea of what you should expect as a result when you add the volute. The difference should not be very large. It is enough to use one impeller blade channel, extend the mesh at the outlet, and use constant pressure as outlet boundary condition.

Hi Conny,

I try this way, but the results in the volute wasn´t good. So I modelled the complete pump (impeller-volute with all the impeller blade channel) and the results in the interface are good in nominal and over load but in part load the difference between total pressure in the turbine inlet and impeller-volute interface decrease and at one point the value in the interface is bigger than that in the turbine inlet. That can´t be posible. The total pressure curve at the turbine inlet in a Press-Flow Graph has a cuadratic form which intersect the origin. For the interface (impeller-volute) the form is the same but th curve must lie under the curve for the turbine inlet.

It is a very good way to modell turbine impeller channels using one impeller blade channel, extended the mesh at the outlet, and use constant pressure as outlet boundary condition. The first modell from the turbine was made so in recomendation from works doing in Norwegen and the results in the efficiency differ only in about 3 point . But now i´m more interested in the tangential velocity (Cu) values in the volute.

Thanks, Conny

Alberto

You are right, the velocities around the impeller inlet shows that the flow recirculate at this zone (in part load). Near the Pressure side from the blade flows to much back to the volute. The Static pressure contours seems to be good. The dynamic pressure (velocity) component from the total pressure is to big in the interface impeller-volute. This because this bach flow to the volute. But I don´t understand why it is so big. It is against the euler equations.

For the pressure calculation I made mass-average pressure (total, dynamic or static) at the inlet and at the interface

Thanks

Assuming that you haven't mixed up reference frames etc. then the problem must be either a numerical problem or a model problem. I have seen this kind of "rising total pressure" effects sometimes with the classical k-epsilon model on Fluent. Switching to a Realizable model or the RNG variant usually helps a bit. Which turbulence model did you use?

(1). I can only say that, Fluent has its way of specifying boundary conditions when using the moving reference frame. Make sure that you have followed the process step-by-step. I had trouble of specifying boundary conditions at the begining a couple of years ago. (2). The only way to find out what's wrong is to check the results by hand. So, from the computed results, go to the inlet (upstream) location and check the static pressure, the velocity at a point. You should have only one static pressure. For the velocity, you have the absolute velocity in stationary reference frame and also a relative velocity in moving reference frame. So, make sure that they are consistent. You can also draw the velocity vectors on the paper. In moving frame, the hand computed inlet velocity must include the rotational speed of the moving frame in the velocity vector calculation. (3). Since you are able to see the flow separation around the blade leading edge, then, you must be using the relative velocity vector in the moving reference frame. This is consistent with your calculation because you are using the moving reference frame. So, use the hand calculation to pick a location and write down the static pressure, and the relative velocity around the leading edge. (4). Now, you can compute the relative total pressure at these two locations,using the static pressure and the relative velocity. (5). At these same locations, use hand calculation to find the absolute velocity in stationary reference frame. Use static pressure and the absolute velocity to compute the absolute total pressure in stationary reference frame. (7). In stationary reference frame, the absolute total pressure should increase through the pump because you are adding work to the fluid. ( there is a slight absolute total pressure loss in the inlet section due to stationary wall loss. there is also a similar loss in the pump passage.) (8) you should check out these numbers by hand because it has confused many engineers working in this area. (since it is not always possible to know whether the number computed is absolute or relative. and sometimes the graphic display does not tell the exact story.) (9) Hope that this will guide you to the answer.

Hello Jonas,

I use k-epsilon. I agree with you it can be a problem from the turbulence model. It is a very good hint. I use k-epsilon RNG, but only in the best operating point and the solutions didn´t differ much. If we modell it at part load operating condition the recirculation are bigger and the effects of rapid strain and streamline curvature can be better represented with RNG.

I will try it.

Many thanks for your good hint.

Alberto

I'd use the Realizable model. My experience is that it is better than the RNG model, which in turn is better than the standard model when you have this kind of problems.

Hello John,

I´m sure it will help me a lot for my simulation. I will follow your recomendations. I do part of the postprocessing with matlab exporting a profile from the total,static and dynamic pressure. I will do the same for Velocity and calculate in Matlab the Total Presurre.

Many thank´s

Alberto

Hi,

If the issue was about total pressure greater than the inlet total pressure, here're my two cents.

Total pressure "can" rise above the inlet (freestream) total pressure depending on the velocityand stress fields, although many would think it's not possible vaguely thinking energy conservation(we always started fluid mechanics class from potential flow and never got to the chapter viscous!

There are many ways to show this. One easy way is to integrate 1-D momentum equation along the streamline. You'll get an equation like Bernoulli's equation but with a additional term involving viscous term, and you'll see what I'm talking about. Depending on the sign of the term, total pressure can rise or drop, although it mostly ends up dropping. Or please read p. 266 of "Introduction to Fluid Dynamics" by Batchelor for an concise explanation. Or professor Issa's paper in one of recent AIAA Journal.

This is not to say that it the total pressure computed by FLUENT with k-epsilon model is correct. In turbulent flow calculations, the turbulent stress field is strongly affected by the turbulence model used. It is well known fact that conventional k-epsilon models tend to overpredict turbulent kinetic energy (outcome of overprediction of production of T.K.E) near stagnation point. And this can lead to overprediction of total pressure. This problem can be ameliorated by using RSM model, realizable k-epsilon model, or RNG k-epsilon model.

Among these, RSM model is the most reliable for stagnating flows. I personally believe that RSM has a lot to offer for tubomachinery flow.

I've also seen this many times - that an overprediction of turbulent energy often leads to an overprediction of total pressure. However, I'm not sure about how this mechanism works - the producion term in the k-equation is exact and even if it is too large to due the underlying incorrect boussinesq assumtion this shouldn't given an unphysical rise in total pressure, right? Or can the increased turbulent viscosity lead to this rise in total pressure? I could understand this if it was only a local pheomenon but I'm quite sure that I have seen it affect the global average also.

What I'm wondering is really if the rise in total pressure follows directly from the overprediction of turbulent production or if it is a secondary problem? And if it is a secondary problem - is it a numerical problem or a model problem? Anyone have any more insight into this?

(1). I have been using the two-equation k-epsilon turbulence model in my own Navier-Stokes code since early 70's, and I was not aware of this problem. (2). When I started using Fluent in 96 for turbomachinery flows, I have noticed that the contour plot had the tendency to extend further upstream of the blade leading edge. I thought, it was due to the accuracy of the contour plot level itself. Sometimes, it is easier to specify the contour level to a higher level, in order to see the picture more clearly. (3). I did not look into the source of this problem further, but I think, one can check out whether it is a function of the local mesh in the leading edge area by simply refine the mesh. (4). In this way, one should be able to see whether the problem is in the inviscid region or in the viscous boundary layer region. (5). It is also a good idea to check out both the incompressible and the compressible modules. ( For the in-house compressible code I am using, the wiggles in pressure field are highly visible at low Mach numbers in front of the leading edge area. As a result, overprediction in static pressure and total pressure are possible. The code uses an algebraic turbulence model. So, it is purely a function of the numerical scheme used in the code. ) (6). I think it is important to identify the source of the problem first, whether it is related to the mesh density, the mesh type, the numerical scheme, or a particular code first. (7). I also remember that it was a function of the particular turbulence model option used. But it is too early to say that there is a direct link between the total pressure increase and the turbulent kinetic energy in a turbulence model. I guess, it is a new field of research.

Hi Jona and John,

As I said in my email, total pressure "can" rise "locally" over free stream total pressure. The phenomea is not unphysical, although many people tend to associate it with energy conservation, concluding it is unphysical. Pleaser read my previous email carefully. Again, this is not necessarily to say that the prediction of the total pressure by engineering turbulence models (k-epsilon in particular) for this particular case is correct. Even though total pressure can locally rise above freestream total pressure in principle, it appears that, for many turbulent flows (leading edge of airfols at incidence, leading edge of bluff ground vehicle, etc.), turbulence modeling can unduly magnify it depending on the local flow and level of turbulence model used . This has been found by many others. As we all know, the production of T.K.E computed by k-epsilon model is NOT exact, and when significant extra rates of strain are involved, k-epsilon models always overpredict the production leading to eventually overprediction of the turbulent and effective viscosity. We found that using Reynolds-stress trasport model greatly helps.

(1). Thank you very much for your response. (2). I am comfortable with the two-equation k-epsilon model and I have not used the Reynolds stresses model before. (3). The point I was trying to make was : whether the total pressure field is directly linked to the two-equation turbulence model? or whether it is a consequence of mesh density and code implementation of the particular turbulence model. And this was not an issue for me before. (4). For the stationary blade calculation, the total pressure should decrease due to viscous loss. On the other hand, for the moving blade calculation, the absolute total pressure (computed in stationary frame of reference) can increase depend on the amount of work done on the fluid by the blade. I think, we are talking about two separate issues here. There is no problem about this part of total pressure increase.

Insufficient resolution may be partly responsible. But I understand turbulence model is llargely responsible for that. In the framwork of isotropic turbulent viscosity, the total pressure along a streamline can be written as;

vec_u * grad H = visc_turb * vec_u * (grad-div (vec_u))

where H is toal pressure

What I was trying to say was, depending on the sign of the inner product on the RHS of the equation, total pressure can increase and the magnitude of the rise is determined by turbulent viscosity. Traditional k-epsilon models overpredicts turbulent viscosity especially near the stgnation points and eventually total pressure as the equation suggests..

(1). Thank you for the formula of the total pressure. (2).Assuming that the free stream is turbulence free ( inviscid flow), then the term " vis_turb" would be zero in the free stream region. Therefore, the total pressure should be constant there. (3). The boundary layer thinkness should be relatively thin at the leading edge ( or at the stagnation point). So, the effect on the total pressure can only occur in this thin layer region based on the above formula. So, if the computed results show a sudden increase ( or decrease) of the total pressure in the viscous stagnation point region, then we can link it to the k-epsilon model. This can be easily verified by setting the free stream turbulence level to a close-to-zero value, and then plot the computed total pressure distribution ahead of the stagnation point. Is this approach reasonable?

Once you've made the bousinesq assumption then the turbulent kinetic energy production term *is* exact, and it exactly matches the energy taken from the mean flow. The problem is with the underlying bousinesq assumption (which is not valid in flows with large normal strain, ie stagnation flows and strongly accelerated regions).

I agree with you that on a streamline total pressure can locally increase due to viscosity and turbulent viscosity. However, this is a local effect and shouldn't affect the average.

My question is really how can an overproduction of turbulent energy lead to a rising *average* total pressure. To me this seems unphysical, yet I have seen it happen several times. Switching turbulence model does affect this so the problem is clearly linked to that. But I suspect that there is a secondary problem here that I can't see. Numerical pehaphs? Or are you saying that the increasing average total pressure is a direct and physical result of a too high turbulent production? In that case I would really appreciate an explanation as to how this happens.