[snoopy]

Hello

I asked about this problem before but I can't solve the problem yet.

I have flow rate 1.37 m^3/s at outlet from an experiment.
I imposed initial conditions as 4.16ATM pressure at inlet but after CFX 11 runned I got a result 2 m^3/s at outlet.
As I told you, I have to have result as 1.37 m^3/s at outlet.
What should I do?
I already checked modeling, scale and fluid properties and so on.

The problem is that there is more flow rate at outlet in cfx than real experiment value.
In my opnion, there is less frictional loss in cfx than real flow?
Do you have any idea for this problem?

Thank you in advance.

Have a nice day.

PS : I attaced outfile. Plelase help me.

[sans]

Hi, Firstly your using Pressure BC's at inlet and outlet which is unreliable (read the manual). Why not use mass flow as a BC and calculate other parameters and validate. Secondly your simulation isnt converged, for these kind of problems you would need your residuals to be less than 1e-4 (closer to 1e-5). Also monitor your variables of interest, let them stabilize.
Start with a lower order scheme and then move up to higher order one for more accurate results.

[snoopy]

Hi

Do you have manual?
I don't know which manual should I see.

About pressure at inlet and outlet, you told me that's unrealistic but that values are from the real experiment. That's why I choose the valuse.

Please give me another advice.

[Abou ali]

Hi,
Did you run a Grid solution dependency to see the grid influence on the solution? If not you must do it and take care of the grid resolution near walls where y+ must be in [20 100] for the k-e model.

For the y+ values you can plot a contour of this variable at walls in the CFX-Post.
To adjust y+ values you must adjust the distance of the first nod near the wall in your masher.

For Grid solution dependency you have to check the solution variation in many grids, coarse grid (ex: 10 000 nods), medium (ex: 20 000 nods) and fine grid (ex: 40 000 nods).

[sans]

Originally Posted by snoopy

Hi

Do you have manual?
I don't know which manual should I see.

About pressure at inlet and outlet, you told me that's unrealistic but that values are from the real experiment. That's why I choose the valuse.

Please give me another advice.

By manual I meant the CFX help files. As an alternative you can use a fully developed flow at inlet and free outflow.

[Attesz]

Hi,

Firstly your using Pressure BC's at inlet and outlet which is unreliable (read the manual)

You are using:
Boundary Type = INLET
Location = INLET
BOUNDARY CONDITIONS:
FLOW DIRECTION:
Option = Zero Gradient
END
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Static Pressure
Relative Pressure = 4.16 [atm]
END

I'm not experienced in simulation of water flows, but i think, inlet pressure must be "Total Pressure" or if you use opening "Opening Pressure". At the outlet, you have to use static pressure. From these values, the solver calculates the other parameters at gases, but i'm not sure it's right for water...

I'm calculating a centrifugal compressor, and I got wrong results by using mass flow outlet.

Regards,
Attesz

[Tristan]

There's no guarantee your simulation will match the experiment. I have an air flow problem where I use a total pressure inlet boundary condition at the inlet and a static pressure opening boundary condition at the outlet. My yplus values are all in the 20 to 100 range as recommended for the k-epsilon model and wall functions. But after all that, the mass flow rate is 10-15% higher than measured in our experiment.

There's only so much you can expect from a RANS simulation that isn't tuned specifically for your application. Then again, who says the experimental data is "right"?

Tristan

[Attesz]

Tristan, I have the same problem, in my cf compressor, the mass flow rate is more lower than measured. What do you think, what's the problem? Maybe with the mesh?