CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Surface roughness setting for a model in wind tunnel test section (http://www.cfd-online.com/Forums/cfx/63098-surface-roughness-setting-model-wind-tunnel-test-section.html)

Sharon March 28, 2009 06:00

Surface roughness setting for a model in wind tunnel test section
 
Urgent!!!!!
do anyone know how to do the setting for surface roughness of model?....the model is tested in a wind tunnel test section...if the roughness tat i get after using the prfilometer is 1.05micrometer, then how can i do to set it for my subsonic simlation?.....plz!!!!Help!!!

Baldy March 28, 2009 23:24

Your turbulence model needs to have a Scalable wall function.

After that, you can enter it in the Boundary Details of the wall.

Sharon March 29, 2009 08:11

ermm...wat u mean by the " to have a Scalable wall function "? where and how can i get it? the "Boundary Details of the wall"....is it during the boundary condition setting?....

Baldy March 29, 2009 12:11

You need to use a Turbulence model that has a Scalable wall function (ie k-Epsilon, RNG k-Epsilon , SSG Reynolds Stress).

When you define your boundary as a wall, click on the "Boundary Details" tab then set the "Wall Influence On Flow" as No Slip. Underneath that you can set the "Wall Roughness" as a Smooth Wall or Rough Wall. Select Rough Wall and then you can set your Roughness Height.

Sharon March 30, 2009 06:42

1 Attachment(s)
but wat i set is based on tutorial since the SST had been used for the simulation ooo.....so, tat means i hav to choose the turbulence model other than SST?....but if i change the turbulence model to eithr k-Epsilon, RNG k-Epsilon or SSG Reynolds Stress...den wil it b any diffrent o incorrect simulation for my model not?....here i m hav attached a print screen file....i dint see any rough wall setting as wat u mentioned..... pls hav a look for me...thx!

Baldy March 30, 2009 11:31

Looks like you have to add manually : http://www.cfd-online.com/Forums/cfx...id-domain.html

Quote:

When using a omega based turbulence model, the roughness option is not visible in pre (at least not in cfx10). You have to manually add it in ccl. Using the SST model (which is omega based at the wall) will hence also not show the roughness option.

If you switch to a k-epsilon model, this option should come up in the wall boundary treatment when switching from smooth to rough wall

Bart

Sharon March 30, 2009 12:48

Is it can be said tat the k-epsilon is for rough surface wall simulation whereas k-w model that is SST is used for a refined surface simulation?...

So, if the statement tat i mentioned above is correct, wic part o whr in cfx 10.0 should i insert(key in) the roughness height for simulation?...

Baldy March 30, 2009 14:06

Quote:

Originally Posted by Sharon (Post 211302)
Is it can be said tat the k-epsilon is for rough surface wall simulation whereas k-w model that is SST is used for a refined surface simulation?...

So, if the statement tat i mentioned above is correct, wic part o whr in cfx 10.0 should i insert(key in) the roughness height for simulation?...

Look up CCL in the documentation. I don`t use them so I cannot help you further.

Sharon March 30, 2009 21:09

oic...anyway, thx for all the info given...it is appreciated!..but, if possible, i would like to look for some1 who ever solved this problem to help me!!!hope can get it! thx....

Timon March 31, 2009 03:27

You just need to add the ccl-section manually. The ccl generated for an adiabatic wall with roughness height looks like this:

BOUNDARY: Yourboundary
Boundary Type = WALL
Location = Yourlocation
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
WALL INFLUENCE ON FLOW:
Option = No Slip
END
WALL ROUGHNESS:
Option = Rough Wall
Roughness Height = RH
END
END
END

Where RH can be a value or a function. So look up your boundary in the ccl and add the "wall roughness" section.

Sharon March 31, 2009 06:19

how can i add in the ccl?..edit it into the command editor for the boundary condition (streamlined body) tat i had created?...

Timon March 31, 2009 07:51

That's an option, although pre might give an error-message then.

Another option is to write the ccl-section in a separate file and use import ccl in pre to load it. Or you can run cfx5solve with the "-ccl file.ccl" option.

Yet another option is to use cfx5cmds to read/write ccl from your command line.

Command "cfx5cmds -read -def file.def -ccl file.ccl" extracts the ccl from your def file, which you can then edit and save. Command "cfx5cmds -write -def file.def -ccl file.ccl" then succesively writes the modified ccl file into your def file.

Sharon March 31, 2009 13:09

ya, there is error msg come out wen i direct edit the command at the command editor.. but i dont know how to write the ccl-section in a separate file as u mentioned above since cfx can be said that is a new simulating software for me n it require time to explore its functions..


All times are GMT -4. The time now is 01:55.