CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   one reference values area. how is it possible? (http://www.cfd-online.com/Forums/fluent/101865-one-reference-values-area-how-possible.html)

OfirLaor May 15, 2012 17:55

one reference values area. how is it possible?
 
Hi all,
When I set the AREA field in REFERENCE VALUES in ANSYS FLUENT, how does FLUENT use this?
The guide says that it is helping with calculating non dimensional coefficients.
However, different coefficients requires different areas…
Drag coefficient area is calculated by the frontal area.
Lift coefficient area is calculated by the span*chord area.

So, is Fluent simply takes the area that the user defines at the REFERENCE VALUES section???
Can someone explain that?

thanks

Mateusz August 23, 2012 16:03

i would know it too, any ideas?? :)

NormalVector August 24, 2012 21:24

Quote:

Originally Posted by OfirLaor (Post 361303)
Hi all,
When I set the AREA field in REFERENCE VALUES in ANSYS FLUENT, how does FLUENT use this?
The guide says that it is helping with calculating non dimensional coefficients.
However, different coefficients requires different areas…
Drag coefficient area is calculated by the frontal area.
Lift coefficient area is calculated by the span*chord area.

So, is Fluent simply takes the area that the user defines at the REFERENCE VALUES section???
Can someone explain that?

thanks

Yes, I believe that's how it works. Computed values such as drag coefficient, lift coefficient, Nusselt number, etc. draw from that "Reference Values" panel. The number you are computing should change if you alter a reference value and then re-compute it.

One way you could handle the different areas needed for Cd and Cl is to use the appropriate area for Cd, calculate it then change to the appropriate area for Cl and calculate it.

Mateusz August 25, 2012 04:35

seriously we have to compute 1 times for cd then change reference area and compute cl??? did i understood correctly?

i have to compute polar for canard configuration (only half wing + horizontal tail) what is my reference area and reference lenght which chord and which area (main wing, tail or main wing + tail?)
, i think there is need to put ref area and ref length for both (wing and horizontal tail) but there i can put only one ref area and ref length

NormalVector August 25, 2012 15:09

Quote:

Originally Posted by Mateusz (Post 378634)
seriously we have to compute 1 times for cd then change reference area and compute cl??? did i understood correctly

I think so, that's the only way I can see using different reference areas/lengths for a report calculation. If someone has a better way I would like to know.

As for which reference values to use for your case, I'm not sure. I don't have too much experience with the non-dimensional aerospace constants. :D

Mateusz August 25, 2012 17:02

today i read several tutorials and i think that chord*span area should be used to compute cl and cd (one ref area to both of them), in 2d causes too (ref area = chord*1). anyway thanks for your interest my problem ;)

NormalVector August 25, 2012 17:28

Sure, no problem. I had to use the Reference Values to compute some Nusselt numbers so that's where I've had some experience with them.

cfd seeker August 26, 2012 03:01

Reference area is just a reference area nothing special to worry about. You can use any area of your geometry as the reference area provided you mention it with your results. If Reference area is not provided with the results then by default its Platform area of the wing i.e chord*span and Reference length is the chord length of your wing or aerofoil. These Refernce values remain same for both Cd and Cl, this convention is fallowed in Aerodynamics. Its useless to run extra simulations for Cd based on some other Refernence area instead you can do other important things :D . These are the rules generally fallowed in aerodynamics but if at all you have to use some other Reference area for drag then in this case also there is no need to run extra simulations instead you can do the fallowing.

1. Calculate Cl and Cd based on the same Reference area say for example Ref1
2. Choose reference area on the basis of which you want to calculate Cd say for example Ref2
3. Then Cd)ref2=Cd)ref1*(Ref1/Ref2) and now you are done

Mateusz August 26, 2012 04:29

thx cfd seeker for your help, your words seems to be known ,the same multiplications of drag we have to do in analytical calculations of drag :)

the same is with calculating moment coefficient cm? but i mean when i calculated it arround axis Y and x-coordinate is x=-1 , but i wat to recalculated it to point x=-2?

cfd seeker August 26, 2012 13:55

Quote:

i mean when i calculated it arround axis Y and x-coordinate is x=-1 , but i wat to recalculated it to point x=-2?
Moment= Force*Moment arm....you can calculate force from moment(moment calculated from fluent) and then recalculate moment around any other point provided axis are same

Mateusz August 26, 2012 15:09

ok thanks :) i have only one more question, can you tell me if value Y+ <1 is good for sst transitional model?? everywhere people write that Y+ should have a value of 1.

Mateusz August 26, 2012 16:02

and one more :) how can i set value of
1.length scale (velocity inlet)
2.turbulent length scale (pressure outlet) and
3.length scale (in pseudo transient Run Calculation).

is1=3?

cfd seeker August 27, 2012 02:56

Quote:

Originally Posted by Mateusz (Post 378764)
ok thanks :) i have only one more question, can you tell me if value Y+ <1 is good for sst transitional model?? everywhere people write that Y+ should have a value of 1.

Yes its very good to have y+ <1. It is also written in Fluent Manual. BTW you are using SST kw woth transition option(2 equations model) or you are using k-kl-w transition model(3 equations model)?

cfd seeker August 27, 2012 03:00

Quote:

Originally Posted by Mateusz (Post 378771)
and one more :) how can i set value of
1.length scale (velocity inlet)
2.turbulent length scale (pressure outlet) and
3.length scale (in pseudo transient Run Calculation).

is1=3?

Default values are generally good enough and also there are no hard and fast rules for these parameter. I generally take length scale=0.4*$($ is approximate boundary layer thickness) for wing and aerofoil calculations.
Quote:

length scale (in pseudo transient Run Calculation)
I have no idea about it

Mateusz August 27, 2012 05:49

hi I am very grateful for your help, i use transition sst (4eqn) model :) . i can't find it out, sometimes people say that length scale should be 0,25c , sometimes 0.0175c, and in user guide that it should be length of airfoil (chord i think)...

cfd seeker August 27, 2012 13:57

Quote:

Originally Posted by Mateusz (Post 378846)
hi I am very grateful for your help, i use transition sst (4eqn) model :) . i can't find it out, sometimes people say that length scale should be 0,25c , sometimes 0.0175c, and in user guide that it should be length of airfoil (chord i think)...

These two transition models(3 equations and 4 equations in Fluent 13 & 14) are very sensitive to wall y+ and wall y+ <1 are generally recommended for these two. I also read somewhere that these models are very sensitive to no. of mesh points in the free stream direction and also the turbulence parameters. So you need to take a lot care while using this model. I have used k-kl-w transition model some months back for validating results of an aerofoil and I was facing problems at higher angle of attacks. Can you please tell me what problem you are solving using this problem?

Mateusz August 27, 2012 18:12

i have to symulate flow arround half model of several canard configuration (half wing+half h.tail) with smooth wing and after that with vortex generators on main wing.

i have Y+=0.6 on wing and Y+=0.4 on h.tail i hope it is enough

Mateusz August 27, 2012 18:22

Quote:

Originally Posted by cfd seeker (Post 378812)
I generally take length scale=0.4*$($ is approximate boundary layer thickness) for wing and aerofoil calculations.

how do you know what is value of boundary layer thickness ??

cfd seeker August 28, 2012 01:44

Quote:

Originally Posted by Mateusz (Post 378990)
i have to symulate flow arround half model of several canard configuration (half wing+half h.tail) with smooth wing and after that with vortex generators on main wing.

i have Y+=0.6 on wing and Y+=0.4 on h.tail i hope it is enough

yes your wall y+ are good but do keep in mind that you should also take care of the growth rate away from the first layer of cells. If there is a large jump in the size then it will ruin your results.
One more question....how do you know that the flow is transitional over wing and horizontal tail?what's the Reynold No?

cfd seeker August 28, 2012 01:56

Quote:

Originally Posted by Mateusz (Post 378992)
how do you know what is value of boundary layer thickness ??

I use formula for flat plate boundary layer thickness(turbulent B.L) and then divide it by an order of magnitude to use it for an aerofoil or wing.
Mateusz if you have time then and enough computational resources then I willl like/suggest you to use different values for "Turbulent Length Scale" and we will try to conclude to what extent it affects the value of drag and lift. I have read some where in a paper that the Turbulence parameters don't affect the lift and drag values but in my experience with k-kl-w transition model "Turbulence Length Scale" was largely affecting lift and drag. I want to counter check it for another case but due to shortage of time and computational resources I couldn't able to do it yet.


All times are GMT -4. The time now is 01:38.