I think

1- check the smoothing mesh of geometry

2- check the BC velocity inlet and pressure outlet (gauge pressure is zero)

3- change the turbulent model

4- The solution must reach to converge (increase the number of iteration)

Federico Caruso You used very strange boundary conditions. Velocity at the inlet ? Are you really know velocity do define it? I think you can not know it. Total Pressure at the outlet? You can not know TOTAL pressure at the outlet .

This is absolutely wrong boundary conditions.

In turbomachinery they usually use

Total Temperature,Total Pressure at the inlet and Static Pressure at the outlet

or Total Temperature,Total Pressure at the inlet and Mass Flow Rate at the outlet.

I think you have to use this boundary conditions.

Hi everybody and thanks for your answers.

To Abbas J Jubear : my mesh quality is quite bad, the impeller is single blade and volute is double curvature (no simmetries at all) and the assembly is gathered from a manufactured version of it so the CAD model is quite generous of slivers, hard and sharp edges etc. Repair does nothing. Turbulent model is realizable k-e, the intention is to go for a k-omega in the future but in literature I found good approximations even with k-e, so I don't think that's the main problem (streamlines do not show separations at best efficiency point), there should be something wrong elsewhere. Probably in the BC.

Hi Vladimir Dorofeev , I have found your answer quite interesting. In many articles that analysed similar phenomena I found BC set as velocity inlet and pressure outlet. So I used the same, but I might be wrong as you said, so I will run a simulation to test it.

Let's say I want to simulate a Head of 11m at 55 l/s. With total pressure inlet, I should insert 107,715 Pa on Gauge total pressure and the same amount at Supersonic/Initial Gauge pressure, right? And then 55 l/s at the outlet as mass flow rate. But then, what should I look at? Should I monitor the total pressure outlet to be 0 or something else?

1- the mesh must be Very soft near the blade surface due to higher shear stress in this region to show the separation point of flow

2-the separation point depends on various reasons such as the velocity of flow, the curved of blade or type of blade ........et

3- check the boundary condition also

Federico Caruso We use this boundary conditions to calculate flow in steam and gas turbines In Ansys CFX.

If I use boundary conditions: Total Temperature, Total Pressure at the Inlet and Mass Flow Rate at the outlet you have Static Pressure at the outlet as main calculated parameter of the flow,so you have to use User Monitor for Static Pressure at the outlet to monitor it diring the solution. When it will be stabilize you get the solution.

If I use boundary conditions Total Temperature, Total Pressure at the Inlet and Static Pressure at the outlet you have Mass Flow rate at the outlet as main calculated parameter of the flow,so you have to use User Monitor for Mass Flow rate at the outlet to monitor it during the solution. When it will be stabilize you get the solution.

You can approach this problem very similar to solving the Bernoulli's equations.

P_total = p_static + 0.5 * H2O_rho * V**2 ; (When inlet and outlet are at the same head). By specifying P_total to be 0.0, you essentially say both p_static and V are zero. This isn't correct.

For turbo machinery, if you are doing a validation study you often have outlet pressure data so try using static pressure outflow first. For a design problem, you most probably have to dig out the enthalpy from the H-S diagram and compute P_total from there. This P_Total is then what you use for the turbo machinery. There will be some uncertainty around P_Total which has to be qualified.

All the best!

The shortest way to sort out this problem is to down load FOAM software is already free source and you can use the application of turbo machinery(pump) that concerning detailed example.

Regards

Hi everybody,

I haven't forgotten about the question, just I took time to run simulations on my local machine which have been quite slow. I followed Vladimir Dorofeev recommendations. I started with tot p_in by inserting at the inlet face pressure inlet BC with only the dynamic pressure of 4858 Pa (3.12 m/s) and pressure outlet 0 with target flow rate 55 l/s. The resulting head was 6m below the experimental data, which was quite disappointing. Then I tried with the other method, leaving the same inlet BC and setting the static pressure outlet to 105757 Pa (10.8m). The resulting flow rate was 20l/s lower than the experimental head at the same operating point (55 l/s).

Right now I am testing different pressure outlet by using the latter method. From what I have understood from Pranav D S about the p_out uncertainty, it is possible that I have to do many attempts by setting different p_out and see how the flow rate behaves. I am thinking that maybe my model does not associate the velocity input to the flow rate that I want, so I have to change the pressure outputs accordingly.

However, if you have better ideas from my experience described above, they are welcome!

I also would like to thank Ahmed Abdelhameed for his answer, however it is mandatory to use Ansys Fluent in this research.

Thank you

Federico Caruso , indeed you have to specify different values p_total to match mass flow rate through your channel. Once you have a match you immediately get a measure of uncertainty in p_total. This can information is helpful when you are computing your losses.

If I understood your setup right, you are calculating an incompressible flow (RANS). According to my understanding then the energy equation is not considered, whereby the temperature and enthalpy is not relevant. So, it's just about pressure and velocity. Therefore, it should be no difference whether mass flow or velocity are given as BC. In addition, it should be incidental at what pressure level you perform the simulation, because the density is constant. You calculate the pump head via the static pressure difference + dynamic pressure difference + geodetic height between inlet and discharge. If the gravity is not considered in the calculation, the geodetic height cancels out. If the pipe diameter at inlet and discharge are equal, the pump head is only calculated via the static pressure difference.

We perform similar simulations and use two different types of boundary conditions (gravity is not considered and pipe diameter at inlet and discharge are equal):

- flow rate at the discharge and total pressure at inlet --> pressure at outlet (or rather pump head) is the result of the simulation

- static pressure at inlet as well as discharge (pump head is prescribed) --> flow rate is the result of the simulation

Of course, mesh quality, convergence and turbulence model are not insignificant! In addition, you should also critically question the measurement data depending on the source:

- Where was the pressure measured? (depending on the position of the sensors, you may need to consider the geodetic height or not)

- Which measurement uncertainty do the sensors have?

Hope you will find a solution for your problem!