CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   FLUENT BUG ?! (http://www.cfd-online.com/Forums/fluent/29514-fluent-bug.html)

S. Ferraris March 16, 2002 13:51

FLUENT BUG ?!
 
Hi !

I have same proble with a calculation with post-processing data. In a 2D model report->suface integral->Area of the total model gives me very bad area (m2) two orders of difference. !!!

Thank you in advance

Sergio Ferraris

venomous March 17, 2002 02:22

Re: FLUENT BUG ?!
 
did you scale the grid after you read it into the solver?

S. Ferraris March 18, 2002 07:29

Re: FLUENT BUG ?!
 
No.

I made the grid in meters and read the same grid , and there was a big difference between the result of the code (~120 m2)and the real area of the 2d model (.5 m2)..

I really dont know what is the problem. But i am trying to find out.

Thank you a lot.

Sergio Ferraris

pp March 18, 2002 07:35

Re: FLUENT BUG ?!
 
Did you check Report-Reference_Values...-Length for second dimension?

S. Ferraris March 18, 2002 08:05

Re: FLUENT BUG ?!
 
Reference value is OK (depth = 1 m)

I was looking more in details and i found that in a 2d model:

In Report - > surface integrals , the values of lengths are OK (inlet-oulet,etc) , but the values of areas are wrong , for example default-interior. This value is correct in Report-> Volumen integral.

I cant get surfaces values in report->surface integral when is a 2D model.?

Thank you

Sergio.

Sergio.

Sundar March 18, 2002 11:21

Re: FLUENT BUG ?!
 
hey,

Just after you export the mesh, make sure your volumes and areas in the case are what you think. If not there is a scale issue or you have created them wrongly. After you run a few iterations, again check flux reprts to make sure the inlet velocity or mass inlet are what you think they should be. So I guess this check will help you to understand where the error is. Sundar

Yvonne March 19, 2002 07:57

Re: FLUENT BUG ?!
 
Hi Sergio! Did you try the same calculation with another Fluent version, too? If you get different results in different versions, call Fluent. If not, probably you did something wrong. I would do the 'version-check'. Others had similar problems and there was indeed a Fluent bug. Good luck, Yvonne

S. Ferraris March 19, 2002 12:48

Re: FLUENT BUG ?!
 
No , i didnt try with other , version because i hacent got it. Indeed is a very easy to prove this bug. Import a 2D mesh (eg 1x1 m) and go report->surface integral->Area ...and yo will not get 1m2..

Thank you .

Sergio

David Shkval March 19, 2002 20:24

Re: FLUENT BUG ?! not bug
 
hey S. Ferraris,

I've solved the problem, it's not a bug. Let me explain in detail.

In fluent, to deal with a 2D case, u should use "Report>Volume Integrals>Volume" to report its area. Though it'll report in m^3, u may set depth=1m to make this value numerically consistent with its area.

If u click on "Report>Surface Integrals>Area", u'll get it's grid's area in Z-axis.

For example, while read in a 1m*1m rectangle mesh(51*51 nodes, say), after set "Report>Reference Value>Depth=1m", u can check volume report and get 1m^3. But while u check surface report, it'll report 98m^2(if interior selected) or 4m^2( boundary selected) or 102m^2 (all area selected). why 102?

(x_nodes51+y_nodes51)*depth1.

Think now u got it.

cya and enjoy!


S. Ferraris March 20, 2002 15:45

Re: FLUENT BUG ?! not bug
 
Thank you. very much !!

So Can I trust the values that Integral Supercies , (eg mass flow rate , etc ) gives me ? I . am not sure.

Thank you again.

Sergio Ferraris

David Shkval March 20, 2002 19:23

Re: FLUENT BUG ?! not bug
 
Yup, Ferraris

mass flow rate, heat flux, etc. are also correct, the keypoint is to use them properly.

Enjoy!

rslgp March 27, 2002 04:46

Re: FLUENT BUG ?! not bug
 
hi, you have nicely solved it, can you solve my problem? as per the mannual the turbulent intensity =u'/U_avg but if ask it plot turbulent intensity you will get only u'( k-e MODEL,STD WALL FUNt.SEGRGATED). It indicate that fluent people are not consitant with their ideas.

IF you use fluent for simulating wall jets, you wont get many of details correctly.I have tried with all models and all bulit in near wall models(like std wall fun., non equlibrium model, two-layer model with different values of K-E model constants, grids spacing near wall, grid adoption using Y* and y+) this indicate that fluent fails to predict many such phenomena correctly.(i have not used fluent-6 yet)


All times are GMT -4. The time now is 19:07.