
[Sponsors] 
November 7, 2012, 03:03 
Delta wing cfd

#1 
New Member
CFDCSD
Join Date: Nov 2010
Posts: 3
Rep Power: 8 
Sponsored Links
I want to know, have i made any mistake in the case setup? what turbulence conditions i need to mention at the inlet velocity boundary condition? I also want to perform simulations with kw SST and kepsilon turbulence models. Is my y+ enough for the simulations with the above mentioned turbulence models? Among all which is a relatively better turbulence model for subsonic CFD simulations of delta wings at high angles of attack? Do i need to make a structured mesh? Your guidance will be appreciated. Best regards 

Sponsored Links 
November 7, 2012, 09:39 

#2 
Senior Member
Join Date: Mar 2011
Location: Germany
Posts: 431
Rep Power: 13 
Few points....
1. I am not clear about your domain, please post a pic. What I got is that your domain is 5 times in all directions which is wrong because downstream your domain should be 15 to 20 times. 2. Running a steady case at such large angles(20, 25, 30, 35) is totally wrong. Large amount of flow separation will take place at such high angles and flow separation is inherently an unsteady phenomenon, so consider running your simulation with unsteady solver 3. What boundary conditions you are using? 4. For turbulence conditions use "Turbulence Intensity" and "Turbulent Length Scale" at inlet 5. Wall y+ 0.1  0.6 is very good for SSt kw and Kepsilon turbulence models but your domain size is very small that's why you have such low wall y+ with only a mesh size of 0.6 million 6. SSt kw model is best recommended for highly separated flows and for boundary layers subjected to adverse pressure gradient. Don't use Standard kepsilon model for your cases because it under predicts separation rather Realizable kepsilon is recommended as compared to standard one. 7. Yes ofcourse structured mesh is much easy for the NavierStokes to handle and it has many advantages as compared to unstructured mesh Hope it helps you Regards 

November 8, 2012, 06:23 

#3 
New Member
CFDCSD
Join Date: Nov 2010
Posts: 3
Rep Power: 8 
Dear CFD SEEKER!
I am grateful of yours for your reply. I have attached the geometry and mesh images. The complete semispherical farfield boundary is taken as Velocity inlet and at the symmetrical circular face of the farfield boundary, Symmetry boundary condition is supplied. The mesh image is depicting the mesh details at the symmetrical face of the farfield boundary. I have read in some literature that for a low subsonic flow taking farfield almost five times the chord length would be enough. Since the Mach no. in my simulation is quite low that's why i have chosen this farfield size. Should i increase it? I am interested in measuring the aerodynamic coefficients. I need to run the unsteady case after the steady case in order to analyze the differences. I have no experience about Turbulence modeling. Can you please suggest me considering my case what values should be given in "Turbulence Intensity" and "Turbulent Length Scale" ? If I use Density based solver and air as Ideal gas with same rest of the flow conditions, will the results remain same as Pressure based? Thanking you again for your time and precious guidance Best regards 

November 8, 2012, 09:51 

#4  
Senior Member
Join Date: Mar 2011
Location: Germany
Posts: 431
Rep Power: 13 
Quote:
Quote:
Quote:
Quote:


November 14, 2012, 22:46 

#5  
Senior Member
Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 151
Rep Power: 6 
Quote:
The turbulence length scale also confused me in the past. When setting the inlet conditions for the calculation of the turbulence scalar quantities there are several different options and I selected intensity and length scales for my analysis of deltawing vortex generators. I estimated the intensity value from the freestream conditions and similar studies in the past however the length scale was a large unknown. I will try what you suggested with the boundary layer however, since my Vortex generators are some distance away from the inlet would it be wise to calculate this boundary thickness at the VGs and use it for inlet 'Turbulent Length Scale'? Thanks for any comments or suggestions.
__________________
 Mechanical Engineering Sydney, Australia 

November 24, 2012, 03:08 

#6  
Senior Member
Join Date: Mar 2011
Location: Germany
Posts: 431
Rep Power: 13 
Quote:
Quote:


November 24, 2012, 07:38 

#7 
Senior Member
Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 151
Rep Power: 6 
I am currently initialising the simulation with a turbulence intensity of 1% at the inlet boundary however, I have more exact values from an experimental study done in the past.
This was in a subsonic wind tunnel and my geometry was based on this so I will try to use it for validation and reference purposes. If I recall correctly, they found the turbulence intensity using Hotwire anemometers and velocity fluctuations in coordinate directions, but I can't remember the exact formulation used.
__________________
 Mechanical Engineering Sydney, Australia 

November 24, 2012, 08:49 

#8 
Senior Member
Join Date: Mar 2011
Location: Germany
Posts: 431
Rep Power: 13 
Yes "Turbulent Intensity" normally comes from the wind tunnel data but from the previous post I inferred that you might have estimated it from some formula which obviously is not the case


November 24, 2012, 08:55 

#9 
Senior Member
Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 151
Rep Power: 6 
What would you suggest for an pressureoutlet boundary condition where backflow turbulence intensity and length scale may be specified in Fluent?
In the past I just set this to the same values as the inlet boundary however, is there a better way of estimating and initialising this based on, for example, some bluff body geometry inside the flow domain? Am I correct in saying that it is entirely possible that the turbulence intensity and the length scale of the backflow might be much larger than the inlet boundary, when vortex shedding is present?
__________________
 Mechanical Engineering Sydney, Australia 

November 24, 2012, 09:13 

#10  
Senior Member
Join Date: Mar 2011
Location: Germany
Posts: 431
Rep Power: 13 
Quote:
Quote:


November 25, 2012, 00:49 

#11  
Senior Member
Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 151
Rep Power: 6 
Quote:
Based on the Fluent Theory Guide, we should use the farfield boundary conditions for a compressible flow however, this is not the case for the M<0.2 and Re=81 000 simulations which I am concerned with.
__________________
 Mechanical Engineering Sydney, Australia 

November 25, 2012, 03:09 

#12 
Senior Member
Join Date: Mar 2011
Location: Germany
Posts: 431
Rep Power: 13 
Ok give it a try and do share your results/experiences here


November 25, 2012, 03:34 

#13 
Super Moderator

For low Mach number, requirements of the farfield increases. For your case flow is also mix of laminarturbulent. For low Reynolds numbers boundary layer is also thick, so make sure you have well resolved mesh covering the whole boundary layer.
For boundary conditions use: 1. Velocity inlet at the inlet 2. Pressure outlet at the outlet. I have recent paper, where someone has simulated the delta wing for these AOA and low Mach using similar meshing (ICEM tetra + prism) and CFX solver. Although it is not of good quality, but it has every thing you need. Just email me if you need it. 

November 25, 2012, 03:59 

#14 
Super Moderator

In old Fluent there were two solvers
1. Segregated 2. Coupled In new Fluent these solvers are renamed to: 1. Pressure based 2. Density based Pressure based solver is used to solve incompressible flows, although you can also solve the compressible flows, but it will have error, as every equation is being solved sequentially: first continuity and then pressure until both velocity and pressure field (continuity and momentum equations) is satisfied and then energy equation is solved and finally turbulence equations are solved. In density based solver all three equations are solved simultaneously (continuity, momentum and energy) and then turbulence field is solved by taking the mean values from the previously solved three equations. Therefore the memory requirement is higher for the density based solver as all three equations should be in the memory. But it is accurate for the flows where the pressurevelocity coupling is strong (compressible flows) and will incur error if solved separately (pressure based solver). There is third solver which is called pressurebased coupled solver based on the Rhie Chow interpolation. Which solves the continuity and momentum simultaneously and then solves the energy equation. At the end it solves the turbulence. So if the pressure velocity coupling is strong and energy equation is not important then the best options is to use the pressure based coupled solver , which is case for your problem. CFX is also coupled pressure based solver, just for your information. If has advantage that it has little more requirement of memory than the pressure based (segregated solver) and very low as compared to density based solver. And it is as accurate as density based solver. In terms of no of iterations, density based solver and pressurebased coupled solver uses very less iteration and pressurebased segregated solver uses more iterations. In terms of memory density based solver uses the almost twice the memory as compared to pressurebased segregated and pressurebased coupled. http://www.cfdonline.com/Wiki/RhieChow_interpolation http://staffweb.cms.gre.ac.uk/~ct02/...is/node17.html 

December 2, 2012, 02:58 

#15 
Senior Member
Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 151
Rep Power: 6 
I finally tried out the boundary conditions using the following turbulence specification settings 
Inlet Specification = 4.5 m/s (same as original) Turbulence intensity = 0.01% Turbulence Length Scale = 0.0019 m Outlet Specifications  Gauge Pressure = 0 Pa Turbulence intensity = 0.01% Turbulence Length Scale = 0.0019 m Note that the calculations were performed as shown below, so please suggest changes if there are obvious mistakes in the approach. The reference plane was taken at the start of the ramp, and Re_x= 500 000 based on 4.5 m/s and the length from inlet of 1.717 m at 25 deg. C ambient air. Boundary thickness = \delta_0.99 = 0.382x/Re^{0.2} = 0.0475 m Boundary layer Length Scale = 0.019 m Turbulence Length Scale = 0.0019 m I reduced the length scale by a factor of 10. The results were actually significantly different to the first steady state simulation and I am attaching the images here from the Cp, Cf and Wall y+ plots. My additional concern is that I have been unable to use the wall shear stress plots or the Cf plots to identify the reattachment or separation point. This is why the normalised velocity u_i/U_0 profile was also attached. This was plotted on wallparallel lines just 0.01 mm off the surface along the longitudinal centreline of the tunnel (NearWall TurbulenceLengthScale.png). Any discussion or ideas shared will help me a lot in understanding this process and I look forward to your replies.
__________________
 Mechanical Engineering Sydney, Australia 

December 3, 2012, 05:11 

#16 
Senior Member
Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 151
Rep Power: 6 
I have been plotting the results after the Fluent data is exported into CFDPost. Currently, I have a basic understanding of the process Fluent Solver uses to calculate the Cf and Cp values and since they are heavily dependent on the reference values I will share them here 
Area = 1 m^2 Velocity = 4.5 m/s (same as my freestream) Gauge Pressure = 0 Pa Density = 1.185 kg/m^3 (same as the rest of fluid domain) I am concerned about the area value in particular. Should this be equivalent to the the surface area of the walls which are of interest? I am only skeptical about this since this surely affects the calculation since Area_ref appears in the denominator for the Cf calculation. Although it is not the most efficient or convenient method, is it more accurate to write scalar variables or expressions for this in CFDPost to extract results for Drag, Cf and Cp? I look forward to all suggestions.
__________________
 Mechanical Engineering Sydney, Australia 

September 19, 2013, 04:41 

#17 
New Member
Join Date: Sep 2013
Posts: 9
Rep Power: 5 
Hi,
I am also doing analysis of a half delta wing. My problem lies in setting the angle of attack. I've defined Total pressure(Stable) at the inlet, and Now it asks me to give flow direction. So, now, in the flow direction wht should I define?? Unit vectors or magnitude of the inlet velocity in X, Y and Z direction. Like if the AOA is 5 degrees, then in Xdirection should I give just the value of Cos 5 or U*cos 5. My flow is in Xdirection and rotation axis is Y. Thanks 

Tags 
cfd, delta wing, fluent, turbulence modeling 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Asking for WI1LSE Delta Wing Geometry File  Dian  Main CFD Forum  0  June 28, 2010 03:00 
CFD of conventional wing with a winglet?  mimi  Main CFD Forum  0  December 7, 2006 10:52 
Delta wing Pitching moment  Riaan  FLUENT  1  March 15, 2005 02:07 
Delta Wing Structured Grid  Riaan  FLUENT  3  December 31, 2004 13:03 
Which is better to develop inhouse CFD code or to buy a available CFD package.  Tareq Alshaalan  Main CFD Forum  10  June 12, 1999 23:27 
Sponsored Links 