Ansys Turbulent Flat Plate: reproducing results published by NASA
 

Dear fellow forum mates,

I am currently doing a project for my 4th year CFD course. My problem statement is a turbulent flat plate. My simulation is based off of the NASA turbulent flat plate.

Nasa Website: http://www.grc.nasa.gov/WWW/wind/val.../fpturb02.html

Now I need some help in finding out where my error lies since after ever single run my skin friction vs reynolds number doesn't match Weigarts Data.

So let me outline what I have done.

For the geometry I decided to draw a box, my initial points (In a XYZ co-ordinate system) is (-0.5x0x0) and my final point is (5.09016x0.328x0.00109). The co-ordinates are in meters. I then used the imprint feature to imprint two surfaces both with a length of 0.5m on the XY and XZ plane to divide the plate up.

Next for meshing I used CFX-Mesh and used edge sizing and bias factors to get a mesh distribution. I used mapped face meshing as well. For the two top edge I set the number of divisions to 200 while for the sides I set the number or divisions to 160 while setting a bias factor of 90. I used named selection, I set the left side edge as an inlet, right side as an outlet, both faces as symmetry, the bottom edge as inviscid for the first 0.5m and viscous for the rest. The top edge was just named top.

For the set-up I set the inlet with the following values: Ux=68.8m/s, k=23.6 and omega=12.83. For the outlet I set it as pressure outlet with the relative pressure as 14.7psi. I set the inciscid as a free slip wall and the viscous as a no slip wall. The faces were set as a symmetry boundary. I am having trouble setting the top edge as I have tried to set it as a free slip wall and even as a symmetry BC but It doesn't change my values. The website sites the top as a freestream BC but I don't know what I should set that in Ansys as. I am using SST for the solving method with a rms of 1x10-6. The operating pressure and temperatures were set as the freestream values of 14.7psi and 540R.

For cfx post I created a velocity vector along the symmetry plane and a pressure countour as well. From the pressure and velocity contours everything seems fine. I drew a line at the outlet and ploted a velocity vs y graph. I then drew a line across the plate where I set my wall. I used custom functions to get values for Cf (using Tau) and Re. But unfortunatly I am still off by a decent margin. At Re 0 Weigart has a CF of 0.5 or so I am getting 0.3, the curve matches perfectly though.

Any help would be appreciated.

Thanks

Have you read the FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

Please post an image of the results you are getting, what you expect to get and your mesh. Also post your CCL and/or your output file.

Hello ghorrocks, I appreciate the time you took to reply. I have read the facts. I have attached the corresponding pictures bellow.

Attachment 43917

Attachment 43918

Attachment 43919

Attachment 43920

My output file saved as a text file exceed the forum limits unfortunately.

If you cannot attach the output file then attach the CCL. It is a small text file.

I assume the first image which shows good agreement between the CFD and Weighardt data (whatever that is) is from a publication and not your work. I assume the second image is your work and shows values about 50% less than the published data.

If this is the case then it looks like you are close, but you need to do careful work to get the simulation accurate. This is a normal part of CFD work. You need to:
1) Do a convergence sensitivity study - does lighter or looser convergence make any difference?
2) Do a mesh size sensitivity study - try coarser and finer meshes in both X and Y directions to find the mesh size you need.
3) Do a time step size check (if transient)
4) Do a boundary condition proximity check - does making the inlet and outlet boundaries closer or further away make a difference?
5) Once you have worked through all those issues you often need to go back to step 1 again and re-check based on the updates of those other parameters. It is an iterative process.

You also need to check you are actually modelling the right thing. You already have a publication which appears to have accurate answers - so did they do anything different to you? Maybe a different boundary condition?

Yes, they set the top boundary to a free stream boundary. I do not know how to do that. Oddly enough if I set the velocity in the skin friction equation to 17.8m/s (which is the free stream velocity for a laminar case) I get the correct distribution? I will try to change the sizing around a bit to see if that fixes the issue. Also if I use the density variable given by ansys it gives a density of 1.8 while in reality the free stream density is 1.025. I am assuming the density given in ansys is the material density and not the flow density? As well searching up a skin friction distribution for a mach 0.2 flat plate actually gives multiple graphs where they would match what I have gotten? If I do a laminar case for the flat plate I get the required distribution by using a freestream velocity of 17.8m/s..its a bit weird.

It is starting to look like your problem is not a CFX accuracy issue but rather understanding exactly what the conditions to model are and the way the Cp is calculated.

Yes my issue is what should the top boundary condition be? The website states to use freestream conditions, while some other documentation sets it to a free sliping surface.

For the freestream bc for the top, do I set it as an opening and insert my Ux and k and omega values?

What actually is a freestream BC in your case? Different people define it different ways.

Also: you can use a totally wrong top boundary condition, and as long as it is far enough away from the area of interest it will not matter. A good choice of boundary condition will allow the boundary to be close, your simulation size to be small and your run to be fast. A poor choice of boundary will require the boundary to be far away, your simulation to be large (as the boundary is far away) and your run to be slow. But both a good and a bad choice of boundary condition will still give accurate answers.

Based on the NASA website, the inlet and top of the plate is exposed to the freestream. The outlet is a pressure outlet and the bottom edge are divided into inviscid and viscous segments. The line used to calculated CF is along the viscous region.

Yes, I guessed that. But what mathematically do you want to impose for the free stream boundary condition.

Keep in mind my last post - you can use a simple boundary (eg a slip wall, or a wall with the freestream velocity as a tangential velocity) but just make your simulation domain larger so it does not affect the area of interest.

I have set it to an wall with Ux=68.8m/s (0.2 mach)

By setting a wall boundary with a tangential wall velocity at freestream drops my skin friction factor by 1/2. I have taken your advice and switched back to a free slip condition. I am still off by that 30% margin regardless of which boundary condition I set the top as. I have varied the mesh and it doesn't really change the distribution (indicating it may have already converged)

But have you changed the proximity of the free slip surface to the boundary layer wall?

Yes the free slip and no slip surfaces are defined on the bottom edge of my plate which is the wall.

You don't seem to understand what I am saying. I will have to explain it more clearly.

For your boundary layer flow you probably have a rectangular box as a mesh domain. The bottom face is the wall which grows the boundary layer and the top face is the free stream boundary. The "proximity of the free slip boundary" I have been referring to is the height of the meshed domain from the bottom wall to the top free stream boundary. When you use less accurate boundaries for the free stream boundary you will need to increase the height so the error from the boundary does not affect the region of interest around the boundary layer on the bottom wall.

Oh I will look into that, so what I did was double checked my boundary condition and checked the symmetry condition and realized I made a mistake and defined a symmetry condition to the first 0.5m of my domain (where I have defined the plate to be 0.5m to 5m in the X direction) So I changed that and now I have a much better value for Cf, but I notice it drop's off faster. What do you recommend?
Attachment 43948

Please show a comparison of what you are getting compared to what you expect to get. Also show your mesh and boundary conditions. Please post your CCL as well.

You tried this before but your mesh did not show the entire domain and you never posted the CCL.

How do I output a CCL file? Sorry I am new to this whole thing. All a learning experience.

The expected results are shown here:
http://www.grc.nasa.gov/WWW/wind/val.../fpturb01.html

I previously attached a picture, I haven't changed the mesh, but mesh encompasses the whole domain.

CCL: In CFX-Pre go file/export/CCL
Results: I was hoping you would overlay your results to your expected results. I do not have time to do this, you will help us out if you do this.
Image: Your comments suggest you have partial faces for some boundaries. Please explain what they are - using an image if possible.

Here is the CCL file

Attachment 43953