Hello,

I think this question might be difficult to answer, but I'm quickly getting gray-haired over this, so I'm hoping for some pointers anyway.

I did a 3d vertex-centered parallel FV solver for the compressible NS and I'm in the process of validating it. One of the things I did was to validate some simple flows (cavity, backward facing-step) against the results of a 2d compressible solver that I have not made myself. I also validated against some analytical solutions (e.g. shock tube). These result were all fine.

Playing with the 2d solver, I tried to calculate the steady flow around a flat plate (ie. infinite strip) and work out the Cd value. I did this by integrating the pressure and viscous stresses over the plate

F = S[p-tau_ij]*n_idS

where p is pressure, tau the viscous stress and n_i the components of the surface unit normal. The Cd value should then be

Cd = F/(0.5*rho_ref*u_ref*u_ref) (*)

where ref-values denote free-stream values. I nondimensionalized my flow variables with the free stream values, which means that the force-value that non-dimensionalizes forces is

F_ref = rho_ref*u_ref*u_ref

So, the Cd value should just be

Cd = rho_ref*u_ref*u_ref*F_nondim/(0.5*rho_ref*u_ref*u_ref) = 2*F_nondim

twice the computed non-dim force. Simulating a steady, laminar Mach 0.2 flow at Re = 4e6 around the plate the solver (NSC2KE) spits out a non-dim force of about 1.24 corresponding to a Cd value of about 2.5. This is way off compared to the "experimental" values I found claiming the Cd value to be in the range 1.17-1.98 depending on Re.

I tried the same flow in 3d and get a non-dim force of about 2.14 yielding a Cd value of more than 4.

In both cases I have used a very fine mesh (which I am happy to provide should anyone be interested); especially in the wall-region. I have also allowed for 20 plate lengths of free space in front of the plate (and to the side in 3d), and 60 plate lengths behind it.

I just don't understand why the values computed by the tried and tested 2d solver do not agree in any way with reference data.

Also - assuming my 3d solver is correct - I don't understand why the 3d results would be so different compared to a similar 2d scenario. Arguably, given the finite plate width in 3d the flow will be significantly different than the idealised 2d plate-flow. I just wouldn't expect that large a difference.

Any comments and thoughts to this post will be appreciated.

Thanks, Martin

Don't you need a reference area in your formula for Cd?

Hello,

Yes, however, and I forgot to mention that, the plate is 1x1 units in 3D and 1 unit in 2D so the area factor is simply 1. But you are right, the formulas for the force unit is rho_ref*u_ref*u_ref*l_ref*l_ref and for the coefficient of drag:

Cd = F/(rho_ref*u_ref*u_ref*l_ref*l_ref)

With lref = 1m you still end up with Cd being equal to twice the nondimensional force.

I think my real question here is why I get seemingly wrong results using a proven code (NSC2KE). This code has been used to calculate lift and drag coefficients and pressure coefficients around NACA profiles by others with success. So either I'm doing something wrong or I'm misinterpretating the results. Or my reference results for the flat plate Cd are incorrect.

Hi Martin,

A few things crossed my mind when I read your post:

-What do you mean by 'infinite strip'? It can't be infinite in the flow direction because the boundary layer has to start somewhere. Maybe you meant semi-infinite and then only integrated the forces from the leading edge to a length corresponding the experiment?

-You have included the pressure in your force equation, but this should have no contribution to the drag on a flat plate aligned with the flow. Did you verify this?

-What are the details of the experiment? I would imagine that it is very difficult to measure the flat plate drag corresponding to the idealized situation you are simulating. They may pick up some pressure drag because of the setup and measurement technique limitations (things that are not accounted for in your simulation). Plus, is the flow laminar in the experiment?

-If I were you I would forget about trying to compare drags and just see if you can match the skin friction coefficient predicted by the Blasius solution. If you want to verify that your force calc routines are working properly, I suggest doing something like a thin airfoil (NACA0012 will work)and show that the lift curve slope is 2pi.

Hope this helps.

Thanks for your reply.

It seems one vital thing I forgot to mention is that the flat plate is perpendicular to the flow. In this configuration pressure drag is really all there is; viscous stresses are benign.

In 2d, by infinite I mean that the plate implicitly is infinite in the unmodelled dimension.

The whole setup is that of a steady compressible laminar flow perpendicular to a flat square plate with side length 1 and thickness 0.1 (thickness being parallel to the flow). I use a second order reconstruction without a limiter and deem steady state to be the point where the residual drops below 10^(-6).

Did you select this case simply for validation purposes or is there additional interest in the results? Because it seems very complicated for validation purposes. At Re of 4E6 the wake has got to be turbulent. I don't know how this will change the pressure on the back side of the plate compared to a laminar flow. It is surprising that you are able to get a steady solution for this case. I would think that you would have significant limit cycles in your force predictions because the flow wants to shed vortices. If your grid is fine enough, I suggest running the case time accurately to simulate the unsteady flow downstream of the plate. I believe this would be tantamount to running a DES since there really is no question as to where the flow is going to separate. The only thing you will get wrong is the skin friction, which is not a factor here because it is only acting in a direction normal to the drag.

Also, I think you need to run this 3D.

Hope this helps.

Thank you very much for your answers. To answer your questions, I don't intend to use this for validation per se. Out of curiosity I wanted to see how close the computed coefficients of drag would get to tabulated values, bearing in mind that the flow is quite complex and possibly beyond what a laminar solver can reliably handle. I was, however, struck by the fact that my 3D solver for this case predicts drag coefficients 2-300 % larger than tabulated values. Thinking there might be a problem with my 3D solver, I then tried the test case in 2D on an independently developed solver, and got very different results, yet still far from tabulated ones.

Over the last few days I did a transient 3D laminar simulation. It confirms what you predict. The forces oscillate. I'm beginning to realize that this case may be to much of a mouthful for my solver. I have recently added the SST k-omega turbulence model. After validating the implementation I will try this test again and see what happens.

My interest in computing drag accurately stems from the real purpose of my solver: to calculate the drag on a rocket at low sub-sonic speeds.

The fact that your drag is higher than the experimental data shouldn't cause you to doubt your code. While the case you are looking at is very different, an example where a laminar simulation predicts higher drag than turbulent is for a circular cylinder or a sphere in a cross flow. In these cases the laminar bl separates early and leads to a high pressure drag. In your case the separation location is clear, but there may be other effects.

I still think doing a thin airfoil is the easist way to verify your force predictions.

Thanks again. I will follow your advice and do some NACA 0012 simulations.