CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

one reference values area. how is it possible?

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   May 15, 2012, 17:55
Default one reference values area. how is it possible?
  #1
New Member
 
Ofir Laor
Join Date: Nov 2011
Posts: 10
Rep Power: 5
OfirLaor is on a distinguished road
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
OfirLaor is offline   Reply With Quote

Old   August 23, 2012, 16:03
Default
  #2
New Member
 
Mateusz
Join Date: Aug 2012
Location: Kraków
Posts: 16
Rep Power: 4
Mateusz is on a distinguished road
i would know it too, any ideas??
Mateusz is offline   Reply With Quote

Old   August 24, 2012, 21:24
Default
  #3
Member
 
NormalVector's Avatar
 
NormalVector
Join Date: Oct 2010
Posts: 72
Rep Power: 6
NormalVector is on a distinguished road
Quote:
Originally Posted by OfirLaor View Post
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.
NormalVector is offline   Reply With Quote

Old   August 25, 2012, 04:35
Default
  #4
New Member
 
Mateusz
Join Date: Aug 2012
Location: Kraków
Posts: 16
Rep Power: 4
Mateusz is on a distinguished road
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
Mateusz is offline   Reply With Quote

Old   August 25, 2012, 15:09
Default
  #5
Member
 
NormalVector's Avatar
 
NormalVector
Join Date: Oct 2010
Posts: 72
Rep Power: 6
NormalVector is on a distinguished road
Quote:
Originally Posted by Mateusz View Post
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.
NormalVector is offline   Reply With Quote

Old   August 25, 2012, 17:02
Default
  #6
New Member
 
Mateusz
Join Date: Aug 2012
Location: Kraków
Posts: 16
Rep Power: 4
Mateusz is on a distinguished road
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
Mateusz is offline   Reply With Quote

Old   August 25, 2012, 17:28
Default
  #7
Member
 
NormalVector's Avatar
 
NormalVector
Join Date: Oct 2010
Posts: 72
Rep Power: 6
NormalVector is on a distinguished road
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.
NormalVector is offline   Reply With Quote

Old   August 26, 2012, 03:01
Default
  #8
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
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 . 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
a_run_91 and Mateusz like this.
cfd seeker is offline   Reply With Quote

Old   August 26, 2012, 04:29
Default
  #9
New Member
 
Mateusz
Join Date: Aug 2012
Location: Kraków
Posts: 16
Rep Power: 4
Mateusz is on a distinguished road
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?
Mateusz is offline   Reply With Quote

Old   August 26, 2012, 13:55
Default
  #10
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
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
cfd seeker is offline   Reply With Quote

Old   August 26, 2012, 15:09
Default
  #11
New Member
 
Mateusz
Join Date: Aug 2012
Location: Kraków
Posts: 16
Rep Power: 4
Mateusz is on a distinguished road
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 is offline   Reply With Quote

Old   August 26, 2012, 16:02
Default
  #12
New Member
 
Mateusz
Join Date: Aug 2012
Location: Kraków
Posts: 16
Rep Power: 4
Mateusz is on a distinguished road
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?
Mateusz is offline   Reply With Quote

Old   August 27, 2012, 02:56
Default
  #13
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
Quote:
Originally Posted by Mateusz View Post
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 is offline   Reply With Quote

Old   August 27, 2012, 03:00
Default
  #14
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
Quote:
Originally Posted by Mateusz View Post
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
cfd seeker is offline   Reply With Quote

Old   August 27, 2012, 05:49
Default
  #15
New Member
 
Mateusz
Join Date: Aug 2012
Location: Kraków
Posts: 16
Rep Power: 4
Mateusz is on a distinguished road
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)...
Mateusz is offline   Reply With Quote

Old   August 27, 2012, 13:57
Default
  #16
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
Quote:
Originally Posted by Mateusz View Post
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?
cfd seeker is offline   Reply With Quote

Old   August 27, 2012, 18:12
Default
  #17
New Member
 
Mateusz
Join Date: Aug 2012
Location: Kraków
Posts: 16
Rep Power: 4
Mateusz is on a distinguished road
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 is offline   Reply With Quote

Old   August 27, 2012, 18:22
Default
  #18
New Member
 
Mateusz
Join Date: Aug 2012
Location: Kraków
Posts: 16
Rep Power: 4
Mateusz is on a distinguished road
Quote:
Originally Posted by cfd seeker View Post
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 ??
Mateusz is offline   Reply With Quote

Old   August 28, 2012, 01:44
Default
  #19
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
Quote:
Originally Posted by Mateusz View Post
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 is offline   Reply With Quote

Old   August 28, 2012, 01:56
Default
  #20
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
Quote:
Originally Posted by Mateusz View Post
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.
cfd seeker is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Second Derivative Zero - Boundary Condition fu-ki-pa OpenFOAM 10 May 1, 2014 16:26
It would be wonderful if a tool for FoamToTecplot is available luckyluke OpenFOAM Post-Processing 165 November 27, 2012 07:54
LiencubiclowRemodel nzy102 OpenFOAM Bugs 14 January 10, 2012 09:53
Simulation of a single bubble with a VOF-method Suzzn CFX 18 October 2, 2009 04:18
Reference Values Help Sham FLUENT 0 February 26, 2005 09:43


All times are GMT -4. The time now is 06:04.