Compared MRFSimpleFoam and Fluent in a centrifugal pump!
 

Hi all,
Recently,I am calculating the hydraulic performance and internal field of a centrifugal pump by using OpenFoam-1.5-dev and Fluent.now,I want to recommend my steps.firstly,I generated the mesh in Gambit,save as ***.msh for Fluent and MRFSimpleFoam,and the numerical method i dopted both in Fluent and MRFSimpleFoam are: standard k-epsilon model, simple algorithm and first order upwind.
Additionally,after setting the initial conditions and boundary conditions and the MRF in OF,I modified the discrete format and the under-relaxation factors as followed:
divSchemes
{
default none;
div(phi,U) Gauss upwind;
div(phi,k) Gauss upwind;
div(phi,epsilon) Gauss upwind;
div((nuEff*dev(grad(U).T()))) Gauss linear;
}


fvsolution:
SIMPLE
{
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;
}
relaxationFactors
{
p 0.5;
U 0.5;
k 0.25;
epsilon 0.25;
}
Compared the result in Fluent and MRFSimpleFoam:
① the residual:
Fluent:
http://www.cfd-online.com/Forums/mem..._residuals.jpg
OF:
http://www.cfd-online.com/Forums/mem...3-residual.jpg
② P and U:
Fluent:
http://www.cfd-online.com/Forums/mem...nt_p_total.jpg
http://www.cfd-online.com/Forums/mem...v_absolute.jpg
OF:
http://www.cfd-online.com/Forums/mem...cture105-p.jpg
http://www.cfd-online.com/Forums/mem...cture101-u.jpg
http://www.cfd-online.com/Forums/mem...2-vector-u.jpg
http://www.cfd-online.com/Forums/mem...r-velocity.jpg
③ the hesad and torque:
fluent: head=28.6m, the torque=161.52
OF: head=26.1m,the torque are as followed:






















viscous torque (wallhgb) : (0 0 0)[Nm];power 0[W]
at last, my problems are:
1.strangely,when I calculated the impeller without the volute,and the head of impeller is only 20m,why it went up after adding the volute?
2.the p in OF is static pressure,dynamic or total pressure? While which is total pressure in Fluent.
3.Is the residual in OF above convergenced?and how to determine whether the result is convergenced?
4. or is there any things will cause the differents?whether is wrong or right in my setup?
Regards,
Yours jennifer

Hello Jennifer.

For steady-state incompressible flows, OF computes (static pressure)/rho. There is a 'ptot' tool in OF to compute the total pressure, I'm not sure but I think it's computing (total pressure)/rho, so you will surely have to rebuild rho * ptot in paraview.

There are several points missing in your analysis, such as continuity residuals, turbulent inlet/outlet conditions, it has a great influence on convergence and results. It seems you are using tets (prisms?) in your mesh, it requires a particular attention concerning the convergence of p and continuity.

I've already performed quite a lot of comparisons between Fluent and OF on steady-state incompressible flows, with excellent results in really close agreements (OF is even a little less diffusive than Fluent).

Regards, Etienne.

hi Etienne,
Thank you for your reply,it’s my negligence to make it clearlier. I used tetrahedron in my mesh. under the 0/U:I give a velocity for inlet ,and give shloud, hub and blades for fixedValue (0 0 0),interface patch for ggi, outlet for zeroGradient;the 0/p: outlet for fixedValue uniform 0;and interface type for ggi,and the other patch type for zeroGradient.
Κ=0.07.ε=0.29for inlet,and I calculate them by the equantion:
http://www.cfd-online.com/Forums/mem...n-equation.jpg
My problems are here:
1. how to give a particular attention concerning the convergence of p and continuity?
2. I use ‘calcPressureDifference’ utility to calculalte the Hydraulic head of pump.the differece of Pressure=InletPressure-OutletPressure
=rho*inletPressure-rho*outletPressure
so before I use the ‘ptot’ utility,the head I calculate is wrong because of the pressure I used is static pressure,is it right?
regards
yours jenifer

Hello,

I am currently working on a 3d impeller/diffuser stage case and have one question.

How did you compute the pump head and efficiency in OpenFOAM?

Many thanks

San

there are two adds-on software which are used for computing rotating machines.here you are:
Attachment 3972
another is torque computation software,but i'm afraid it is too large enough to upload,because it displays" 708.7 KB bytes exceeds the forum's limit of 97.7 KB for this filetype".So,would you like to give me your e-mail ,please? i will give you as soon sa possible!
good luck!
your jennifer

Your residuals plots show the slope of the residuals is not zero in both FLUENT and OpenFOAM, so the solution is still changing. Strictly speaking, for a steady state simulation, you might want to compare the results you obtain when residuals stop lowering (the residual plots become flat).

Hi Jennifer,

Thanks for your quick reply, I will send my email address now.

Also I have been trying to get my case to convergence but without any luck.
Could you kindly take a quick look at my case settings also?

I'd really appreciate it.
Regards,

San

I'd like to!

Thanks for kindly accepting.

Here is my case:

- I use MRFSimpleFoam with ggi interface
- The periodicity of the impeller/diffuser is different (6 and 7 passages, repectively) and I understand the limitations of running a frozen rotor case. However my aim here is to just confirm that convergence can be reached.
- I have not impletemented any turbulence right now.


Problem:

I cannot seem to reach convergence further than shown in the plot below. I have played around with different schemes, solver algorithms and BCs with no luck.

I have also tried a case with very slow impeller rotation (designed is 1000 rpm but tried 10 rpm) and then the solution converges with physically feasible solution - Thus I am also suspecting the possibility of it to be a more fundamental problem with the rotational reference frame, ggi interface, etc. Though have not yet found any solution.

Here are some of the visualization and the residual plot:

Attachment 3991

Attachment 3993

Attachment 3994

Attachment 3996


Schemes:
Solvers:
BC Pressure:
BC velocity:
Any suggestions and help are welcome and appreciated.

Many thanks,

San