[H_R]

I am trying to perform a CFD simulation of a 70 degree sweep Delta Wing at different angles of attack (aoa = 20, 25, 30, 35 degrees). The inlet flow is at 25m/s. I have made a spherical Far-field boundary with the sphere radius of 5 times the root chord length of the delta wing. Because of the symmetrical shape only half of the delta wing and spherical far-field boundary is considered for meshing. I have made 10 inflation layers on the delta wing surface to capture the boundary layer and an unstructured mesh in the far-field using ICEM-CFD. A mesh with 0.7 million cells has been created. Since the Mach no. is low, I have run a steady state Pressure based simulation using SA turbulence model in Fluent. Density of air is taken as constant. The hemi-spherical boundary is taken as velocity inlet and the symmetry is applied at the symmetrical face. My y+ lies in the range of 0.1 - 0.6.

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 k-w SST and k-epsilon 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

[cfd seeker]

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 K-epsilon 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 k-epsilon model for your cases because it under predicts separation rather Realizable k-epsilon is recommended as compared to standard one.

7. Yes ofcourse structured mesh is much easy for the Navier-Stokes to handle and it has many advantages as compared to unstructured mesh

Hope it helps you
Regards

[H_R]

Dear CFD SEEKER!

I am grateful of yours for your reply.

I have attached the geometry and mesh images. The complete semi-spherical far-field boundary is taken as Velocity inlet and at the symmetrical circular face of the far-field boundary, Symmetry boundary condition is supplied.
The mesh image is depicting the mesh details at the symmetrical face of the far-field boundary.

I have read in some literature that for a low sub-sonic flow taking far-field 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 far-field 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

[cfd seeker]

I have read in some literature that for a low sub-sonic flow taking far-field 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 far-field size. Should i increase it?

It should be five times of body length ahead of wing and atleast 15-20 times of body length downstream of wing. Yes you should increase it downstream of wing.

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.

Run the steady case for few hundred iterations and then switch over to unsteady case

Can you please suggest me considering my case what values should be given in "Turbulence Intensity" and "Turbulent Length Scale" ?

Turbulence Intensity is usually known from the wind tunnel data but if you don't have wind tunnel data then 1% is ok. For Turbulent length Scale use this formula L=0.4*$(where sigma is boundary layer thickness). For boundary layer thickness use Flat plate formulas to calculate and then reduce it by an order of magnitude to have a good approximate for the wing

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

Pressure based solver is used for in compressible flow while density based is used for compressible. Your case is incomprehensible but this thing doesn't matter a lot except the convergence rate

[Crank-Shaft]

Originally Posted by cfd seeker

Pressure based solver is used for in compressible flow while density based is used for compressible. Your case is incomprehensible but this thing doesn't matter a lot except the convergence rate

I think you mean incompressible flows are suitable for the pressure-based solver however, the compressible flows are generally analysed using the density-based solver.

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 delta-wing vortex generators. I estimated the intensity value from the free-stream 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.

[cfd seeker]

I estimated the intensity value from the free-stream conditions and similar studies in the past

Can you explain how?

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'?

Yes

[Crank-Shaft]

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 sub-sonic 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 Hot-wire anemometers and velocity fluctuations in coordinate directions, but I can't remember the exact formulation used.

[cfd seeker]

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

[Crank-Shaft]

What would you suggest for an pressure-outlet 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?

[cfd seeker]

What would you suggest for an pressure-outlet boundary condition where backflow turbulence intensity and length scale may be specified in Fluent?

Sorry I never used pressure-outlet boundary condition rather I put my boundaries far away from the body and use pressure far-field boundary condition

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?

You seems right logically but I am not sure

[Crank-Shaft]

Originally Posted by cfd seeker

Sorry I never used pressure-outlet boundary condition rather I put my boundaries far away from the body and use pressure far-field boundary condition


You seems right logically but I am not sure

Based on the Fluent Theory Guide, we should use the far-field 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.

• Pressure outlet boundary conditions are used to define the static pressure at flow outlets (and also other scalar variables, in case of backflow). The use of a pressure outlet boundary condition instead of an outflow condition often results in a better rate of convergence when backflow occurs during iteration.
• Pressure far-field boundary conditions are used to model a free-stream compressible flow at infinity, with free-stream Mach number and static conditions specified. This boundary type is available only for compressible flows.
• Outflow boundary conditions are used to model flow exits where the details of the flow velocity and pressure are not known prior to solution of the flow problem. They are appropriate where the exit flow is close to a fully developed condition, as the outflow boundary condition assumes a zero normal gradient for all flow variables except pressure. They are not appropriate for compressible flow calculations.

I will try to specify and initialise using the Intensity/Length-Scale method and compare with some of the others for my own understanding. The backflow specification will be kept identical to the inlet conditions, if they are determined from the characteristic length at the bluff body or the delta-wing.

[cfd seeker]

Ok give it a try and do share your results/experiences here

[Far]

For low Mach number, requirements of the far-field increases. For your case flow is also mix of laminar-turbulent. 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.

[Far]

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 pressure-velocity coupling is strong (compressible flows) and will incur error if solved separately (pressure based solver).

There is third solver which is called pressure-based 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 pressure-based coupled solver uses very less iteration and pressure-based segregated solver uses more iterations.

In terms of memory density based solver uses the almost twice the memory as compared to pressure-based segregated and pressure-based coupled.



http://www.cfd-online.com/Wiki/Rhie-Chow_interpolation

http://staffweb.cms.gre.ac.uk/~ct02/...is/node17.html

[Crank-Shaft]

Originally Posted by cfd seeker

Ok give it a try and do share your results/experiences here

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 wall-parallel 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.

[Crank-Shaft]

I have been plotting the results after the Fluent data is exported into CFD-Post. 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 free-stream)
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 CFD-Post to extract results for Drag, Cf and Cp?

I look forward to all suggestions.

[fender26]

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 X-direction should I give just the value of Cos 5 or U*cos 5.
My flow is in X-direction and rotation axis is Y.

Thanks