CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   Setting the Reynolds number (https://www.cfd-online.com/Forums/cfx/94874-setting-reynolds-number.html)

 Echidna November 28, 2011 21:40

Setting the Reynolds number

I am currently making an analysis of a dual-element wing in CFX.
The problem is that i cannot set my intended Reynolds number so i will have accurate results. I will describe below what exactly i do to see if there is something i am doing wrong.

Re=67778 x speed x length
In my example the length is the chord of the wing which is 0.32m and the speed of the air is 50m/s, so

Re=1.084e6

I leave the operating pressure of the fluid at default (1atm) but then the Reynolds number of the fluid is, according to the solver, 1.34e7.

How can i set the Reynolds number of the fluid?
Thanks a lot!

 Lance November 29, 2011 04:06

The Reynolds number that is given in the output from the solver uses a length scale that is (domain volume)^(1/3) and not the cord length.

 Echidna November 29, 2011 06:10

Quote:
 Originally Posted by Lance (Post 333901) The Reynolds number that is given in the output from the solver uses a length scale that is (domain volume)^(1/3) and not the cord length. Does that solve your problem?
Does this affect the accuracy of my analysis? If yes, how can i solve it?
How can i "tell" the software that the length of interest in my analysis is the chord length and not the cubic root of the whole domain volume?

 ghorrocks November 29, 2011 07:21

The display of Reynolds number in the output file is for the information of the user only. It is not used in the solution at all. Ignore it.

 Echidna November 29, 2011 07:30

Quote:
 Originally Posted by ghorrocks (Post 333936) The display of Reynolds number in the output file is for the information of the user only. It is not used in the solution at all. Ignore it.
OK thanks!
So, it will be sure that the Reynolds number used by the solver will be the one i need? I set the reference pressure at default (1 atm) and air ideal gas as the fluid.
My solution is low speed (50m/s). Do you think it is correct to set the operating pressure at 1atm? I also set the average static pressure at the outlet at 0 Pa, as is done in WS02:Airfoil tutorial.
Thanks a lot for all the help!

 ghorrocks November 29, 2011 17:17

CFX is a dimensional solver, it does not non-dimensionalise the equations so any talk of Reynolds number is purely for the user only. The equations are solved in metres, seconds and kilograms (or any other consistent unit set).

You normally set the reference pressure to be the base pressure (either the inlet or outlet pressure) in a simulation, and use 0 pressure for that boundary. This is good practise.

 Echidna November 29, 2011 19:11

So you think that by setting the reference pressure to 1atm is a good practise for my simulation? The fluid velocity is 50m/s. After reading the WS02:Airfoil tutorial, i found out that you will have to calculate the reference pressure of the simulation, but only if there is any compressibility effect. In my analysis, the speed is low, so there is not any compressibility.
Do you think that it's correct to set the reference pressure to 1atm and the average static pressure (relative pressure) on the outlet at 0 Pa?

 ghorrocks November 30, 2011 05:54

It is a good idea to use a sensible reference pressure regardless of whether the flow is incompressible or compressible. In your case a reference pressure of 1 atm seems sensible.

 Echidna November 30, 2011 06:33

Thanks a lot!

 All times are GMT -4. The time now is 13:52.