CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   STAR-CCM+ (http://www.cfd-online.com/Forums/star-ccm/)
-   -   Radian fan (http://www.cfd-online.com/Forums/star-ccm/93537-radian-fan.html)

cfdivan October 18, 2011 11:47

Radian fan
 
Hi,

Im trying to simulate the performance of radial fan to match supplier values.

Im using Star-CCM+. Simulation conditions are as follows:

Numerical model
MRF
Segregated
Turbulent
kW SST
All y wall treatment

Flow conditions
inlet - stagnation inlet (0 Pa total pressure)
outlet - mass flow (-1.092 kg/s)
blades rotation rate - 2423 rpm

Initial conditions
Pressure (0 Pa)
TI (.03)
Length scale (.004)
Tubulent velocity scale (0 m/s))
Velocity (0 m/s)


Mesh
785600cells
11 prism layers
4mm of prism layer thickness

Im trying to compare the pressure rise for different flow rates for fixed rotation speed but the results don't correlates.
I assumed that the pressure rise is the difference between the pressure at interface of impeller outlet (green) and pressure at interface of impeller inlet (brown).
I very much appreciate your help!

Thanks in advance,
Ivan

http://www.cfd-online.com/Forums/E:\geometry.jpghttp://www.cfd-online.com/Forums/E:\geometry_1.jpghttp://www.cfd-online.com/Forums/E:\volume_mesh.jpg

abdul099 October 20, 2011 08:31

How big is the difference?
Is your mesh fine enough to get a mesh independent solution (I assume, it's not)? Does your mesh look well? Are your interfaces and outlet faces far enough from your fan for the flow to settle down again?

And the most important: Have you ever heard, a MRF simulation is a big simplification of your fan and will never give exactly the same numbers like a (more precise) transient simulation? Just take a few seconds and think about the difference - MRF doesn't consider the history of the flow as it is a steady simulation.

First of all I would check the mesh, as this low numbers of cells with 11 prism layers usually means, the mesh is very coarse. And when the mesh is fine even with this low cell count, I would run a transient simulation, but don't forget to check the position where you set up the pressure reports.

cfdivan October 20, 2011 10:04

Hi abdul

Thak you very much for your support!

The difference is enormous (above 30% in pressure rise). When I increase the flow rate until (4750 m3/h) the difference could reach 70%.
I runned this simultaion in transient regime and the difference still there.

I forgot to share the pictures. Hereby follows
http://img163.imageshack.us/img163/807/testrig.th.jpg

http://img577.imageshack.us/img577/6581/impeller.th.jpg

http://img217.imageshack.us/img217/2...umemesh.th.jpg

The pressure measurements were done in brown and green areas. Do you agree with this approximation? The inlet pipe length is 0.6m a outlet pipe have 1.0m of length.

The boundary values looks fine for you?

Thanks in advance!

abdul099 October 20, 2011 21:55

In my opinion, the faces where the pressure measurement is done is too close to the rotor.
Also the mesh is somewhat strange. I don't understand how you got this low cell count with that much prism layers but having a too coarse mesh.
Also in the last picture one can see, it's too fine to the outlet and too coarse just before the extrusion. Also in the inlet pipe, the cells could be coarser to save some cells which can be invested somewhere else. The cell size growths very quick, right near the rotor. That are some things you could improve.

When running in transient, did you switch to rigid body motion or did you just run that MRF case transient? Did you choose an appropriate time step?

cfdivan October 21, 2011 04:53

In trasient simulation I tried with RBM numerical model with correct time step.

The pressure measurements were done in surfaces reffered in way to match the definition of turbomachinery (energyzing the fluid from inlet to outlet).

I have to agree that the mesh is not good enough (low cell counts) but Im trying to run in cluster.

Once the reference pressure (pr) is 1.013e5, do you agree that the total pressure speficfied (stagnation inlet boundary type) should be zero? or need i to specify the dynamic pressure, i mean
pt=ps+pd

pt - total pressure
ps - static pressure
pd - dynamic pressure

Assuming that ps=pr, hence pt=pd

Have you ever run simulations like that and the results obtained match in accordance with supplier specifications?

Thanks in advance,
Ivan

abdul099 October 22, 2011 22:46

I never had to run a turbomachinery case, especially no fan. I usually did the opposite and run wind turbines. Somehow related, but requirements are different.

But I would say, check your pressure definitions. Pressure probes are usually measuring the static pressure, so your inlet definition should also reflect this. Energizing the flow means, you increase the total pressure, not necessarily the static pressure. Did you consider this in your reports?

Next point: Ever heard about a mesh independent solution? If there's a mesh independent solution, there also has to be a mesh dependent solution. That means, your solution depends on the mesh resolution and changes when changing the mesh.
So give it a try and refine your mesh and look what happens.

Cheers

PS: By the way, what is "the right" time step? How did you obtain the certainty it's "the right" time step?


All times are GMT -4. The time now is 02:46.