Hi!

I have written a 2-D incompressible Finite-Volume code for the computation of flow passing airfoils (using Clark-Y foil) with/without ground effect. My problem happened in the prediction of pressure at the stagnation point near L.E.

When the Re number is as lower as one thousand (Re=1000, based on the chord length), the pressure value (Cp) at the stagnation is over-predicted (about 10% larger than unity, that is Cp_stag ~ 1.1 > 1.0). The flow field approaches to be a steady solution (NOT an oscillation one).

If Re=10^4 or 10^5, then oscillation solutions with vortices shedding are met. The Cp solutions at stagnation points are oscillating around the unity value.

If Re is more over increased to 10^6 or a higher one, the over-prediction of pressure at the stagnation point disappears and the result becomes reasonable.

Can anybody body share experiences about the calculation of LOW Re number flow passing an airfoil or any blunt body? Is it always a problem to predict the pressure distribution in a LOW Re number flow? Thanks for any words!

wowakai

(1).You said you have written a 2-D incompressible finite-volume code for the computation of flow passing airfoils. Then you went on telling us these interesting results. (2). Since you are running your own code, you must know what you are doing. I must say that you are telling us the truth and it is coming from your code. (3). Flow over a cylinder, flow over a square cavity, flow over a back-step, are standard test cases for CFD code validation. This is because there are many papers published and one can find these results easily to validate his code. (4). Without knowing what you have been doing, I would strongly suggest that you pick up some of these test cases and related papers, and do a step-by-step validation of your finite-volume code. Follow some text book examples would be the ideal way to learn the CFD programming. (5). How did you handle the meshes and turbulence models when covering flows with Reynolds numbers form 1000 to one million ?

Dear Dr. Chien,

Thanks for your response! I always learn much from your posting messages in this forum!

I have checked my N-S code by calculating several flows, including 1)the semi-infinite flat plate(have a good match with the Blasius solution) with a uniform inflow, 2)an isolated single airfoil case(DSMA671 airfoil;Re=1.2 mill.)(have got a good solution matched with the experimental data supplied in ERCOFTAC Fluid Dynamics Database), where the used turbulence model is the Smagorinsky Constant-coefficient Sub-Grid Scale LES.

The used mesh for airfoil calculation is multi-block(inner and outer blocks) and C-type. The mesh is established from the streamlines and potential lines of a potential solution solved by using the conformal mapping method. Hence the mesh is smooth and seems orthogonal.

I have tried to find any possible factor that leads to the problem in the LOW Reynolds number flow calculation. Of course, both of fine and coarse meshes have been used for a check. But it doesn't show any different result.

The only difference happens when I increase the Re number, then the over-prediction of pressure in the stagnation region near L.E. can disappear.

In my code the mass of conservation is considered in each cell, and some level of numerical error should exist because of my limited computer resources. The boundary conditions in the far downstream are chosen of constant gradient conditions. Maybe my problem is caused from a violation of global mass conservation.

Regards,

wowakai

(1). If you are getting overshoot in total pressure, you need to look at the total pressure, the static pressure and the velocity field distribution. ( if the formulation is compressible, you need to look at the density field distribution also). (2). The field distributions should tell you whether you have wiggles (oscillations) in the pressure distribution or not. And you should be able to isolate the source of overshoot. The total pressure is a derived parameter, and it should be related to the primitive variables in your formulation. Since the velocity has to go to zero in the stagnation point region, the overshoot can only come from the pressure field. (3). So, it looks like that you have something funny going on in your static pressure field. (4). The Reynolds number of 1000 is not really very low in getting the viscous effect. The viscous effect normally will create more total pressure loss. (5). It is either related to the way you derive the total pressure, or connected to the method used in the code for the pressure field. (6). What is your 2-D formulation? (7). Since you are quite capable of writing the code, why not try to use a different scheme in the formulation to see whether the problem is still there or not. (8). In 2-D, you can calculate flow over a finite plate, normal to the flow. In this way, you can check the static pressure, and total pressure field easily, since there will be a stagnation point in the middle of the plate. (9). I would say that your 2-D formulation is giving you oscillating pressure field solution. That is just my guess. I have no idea about your formulation.

At stagnation point, velocity is zero theoritically and pressure is maximum for momentum and energy balance. Vortex shedding increases drag on the surface and the stagnation temperature increases due to friction increase caused by increase of drag. Cp is a function of temperature if the temperature changes. I guess it may be the reason why Cp value is oscillating around Re = 10^4 to 10^5.

Dear Dr. Chien,

Your descriptions gave me new thought to check the total pressure field distribution in my calculation.

The conventional wall boundary condition for static pressure is to take a zero value of normal pressure gradient along the surface, that is dP/dN=0. It is really the case for "the laminar boundary layer flow" and for "a potential stagnation flow". But for a stagnation flow with evident viscous effects(lower Re number), what will be the suitable wall B.C. for pressure?

Because of this question, I had supposed that the happening of pressure overshoot in my calculation is caused from the use of the condition dP/dN=0. Hence I have modified it in my code and have adopted introducing the full N-S equations to constrain the pressure variable along the airfoil surface. Then I thought it should be the most accurate B.C. for pressure, which I can use. I had been cheered to see some changes.

But the new computational results have shown me the same story. The pressure overshoot didn't change at all.

I know that it is a strange to see the existence of an overshoot total pressure zone. But note that it can be met only when the Re number is lower. Might the tip-nose zone receive additional energy from the nearby viscous boundary layer? Could it be a physical phenomenon?

I think the term "mu( d2(Uj)/(dXi dXi) )" might have some magic effects(can increase energy to the flow) in the tip-nose zone when the developing boundary layer(near the L.E.) is thick enough to do these effects.

For example, the term d2(u)/(dy2) is always NEGATIVE(diffuse the energy) for the laminar boundary layer flow of the Blasius solution. But in the tip-nose case a similar term might be POSITIVE and can then increase energy to the flow.

Excuse me! But I would mail you some plots (mesh, velocity vector, static and total pressure contours)(two *.ps files with the sizes 24K+30K) for a detail show. I apologize that I didn't get your agree at the first. You understand that people can not wait to know or to learn a fact. Thanks!

Best Regards,

Wu Chun-Kai

(1). Please don't invent new physics. What you are getting comes from your own code. (2). Please go through your governing equations, formulations and the code several times to find the hidden bugs. It is very effective if you do this with a friend who is not familiar with your methods. (3). If you are not getting the overshoot at high Reynolds numbers, it is likely that the viscous terms are not formulated properly, and the sign could also be wrong. It is hard to tell because I don't know what you are doing with what equations and formulations. I would say the error is deep in your formulation and equations. So, take your time to check the equations.

Your differencing is unlikely to have been arranged to conserve total pressure and it is quite usual to see these sorts of violations caused by numerical error. In fact, with an incompressible code predicting a stagnating plane jet in a rectangular region one can get an analytically correct velocity field but a pressure field subject to numerical error.

Have you repeated the calculations on a sequence grids where you double the number of grid lines in each direction?

I believe you are using a coordinate system aligned with the streamlines rather than wrapped around the blade? This would usually place strongly distorted cells in the region of impingement. If there is something wrong with the fiddly cross terms in the diffusion terms it would be emphasised here. Can you wrap the grid around the blade to remove this source of numerical error?

dp/dn = 0 is a robust boundary condition for a wall but is, unfortunately, physically incorrect. One cannot simply use the N-S as a boundary condition since you must supply some information on the conditions at the wall.

On a related note, how do you handle your diffusive flux at the wall? What does it transport into/out of the solution region?

Another source of this sort of grief is the pressure smoothing scheme. What are you using? How are you handling the evaluation next to the wall where pressure values are needed beyond the wall?

Are you using a turbulence model? If so, which?

Although you are broadly correct in the assumption that overshoots and undershoots in total pressure may be physically correct there needs to be a simple physical mechanism to achieve it. You are seeing a 10% increase in total pressure above the free stream value (i.e. not in a small back water somewhere). This is too much to be extracted from the turbulence and would have to be transported. At low Reynolds number the transport terms become larger but, unfortunately, so does the dissipation term and this always acts to progressively reduce the total pressure. Where can this amount of mechanical energy come from?

(1). I have received your e-mail of contour plots and mesh. (2). Try to solve 2-D flow through a 2-D channel at Re=100, 400, 1000. (3). Try to solve fully developed 2-D channel flow at Re=100,400, 1000. using the same 2-D code. (4). Check the velocity profiles, static pressure distributions, and compute the total pressure distributions. (5). Always check the inlet conditions to see whether it is consistent with the specified values. (6). Hope you can locate the bugs soon.

Thanks Dr. Chien and Andy!

I reviewed the "Fundamental Mechanics of Fluids" by I.G. Currie. You are right!

In the book in page 32, it is proved that the dissipation function always works to increase the irreversible energy of an incompressible flow. It is also the reason why the total pressure of a laminar boundary layer flow can always be decreased.

In my case, for a steady incompressible flow field near the L.E., it should not exist such an overshoot of total pressure. I am interested to know what happened in the stagnation flow region of larger viscosity.

I have been trying to find the deep bugs, but I didn't succeed till now. I will slove the bugs and will talk to you what had happened to me. Thanks!

Regards,

Chun-Kai

The transport equation for mechanical energy consists of terms apart from T:del(V) which, as you rightly state, is a pure sink for Newtonian fluids. These other terms can locally overcome the dissipation function and increase total pressure though not globally without an external source of work.

Hi,

Total pressure overshoot can happen in many viscous flow problems including the stagnation flow you mentioned. Please take a look at p.266 Batchelor's boog "Introduction to Fluid Mechanics" Incidently, there was an AIAA J. article on this issue and I recall professoe Issa showed, using stagnation flow as example, that totoal pressure overshoot is NOT UNPHYSICAL at all.

Dear Andy,

I have just found theories about the "creeping flows or the Stokes flows(Low Reynolds number flows) in the book "Incompressible Flow" by Ronnld L. Panton, second Ed., 1996. Some statements in the Chapter 21 with a topic "Low Reynolds Number Flows" are shown in the following:

p.686 Chapter 21.9 FLOW OVER A SPHERE

"The streaming motion of a flow over a body when the

Reynolds number becomes small has some interesting

but complicated characteristics. At infinity the

uniform stream has no vorticity, but as Re-->0

viscous diffusion is dominant and SENDS VORTICITY

far from the body. The analysis of these flows

produces a singular perturbation problem where the

singularity is at infinity. We will find that the

consequence of the singular behavior is SEVERE FOR

TWO-DIMENSIONAL FLOWS but relatively benign in

THREE-dimensional flows."

p.688-689

"The pressure reaches a MAXIMUM at the forward

stagnation point and a minimum at the rear

stagnation point. The values are

P - Pinf. = (+-) (3/2) mu*U/r (21.9.9)

This equation illustates the fact that the pressures

in a given velocity field INCREASES directly with

the viscosity of the fluid. For comparison we may

cast Eq.21.9.9 into the form of the pressure

coefficient

(P - Pinf.)/((1/2)ro*U^2) = 6 / Re (21.9.10)

Although this nondimensional form is only

appropriate for moderate or high Reynolds numbers,

it reveals that LOW REYNOLDS NUMBER EFFECTS CAUSE

THE FORWARD STAGNATION PRESSURE ON A SPHERE TO

BECOME MUCH LARGER THAN IDEAL FLOW VALUE OF UNITY.

I carefully tested my code but the overshoot of total pressure always exists in the forward stagnation point region when ReC=1000(based on the chord length). It means that Re|nose~10 for my single airfoil calculation.

Is it possible that I just meet the "creeping" flow or the Stoke flow in my short local farward stagnation flow field?

I would like to show you two plots (mesh, velocity vector, static and total pressure contours)(two *.ps files with the sizes 24K+30K) for a detail description. I apologize for causing any inconvenience to you!

Best Regards,

Wu Chun-Kai

Hi!

I have found some published results about a flow over a CYLINDER.

In the book "Incompressible Flow" by Ronald L. Panton, 2nd ed., 1996., the pressure distribution over a cylinder from the N-S computations of Fornberg(1980) shows us that the maximum Cp at the forward stagnation point of the cylinder varies with the its Reynolds number. Some relative values are shown in the later:

1) Re=200 --> Cp|stag.~=1.01 2) Re=100 --> Cp|stag.~=1.03 3) Re= 40 --> Cp|stag.~=1.14 4) Re= 20 --> Cp|stag.~=1.28 5) Re= 10 --> Cp|stag.~=1.48 6) Re= 4 --> Cp|stag.~=2.00 7) Re= 2 --> Cp|stag.~=2.70

In this case, for a LOW Reynolds number flow it is possible to have a pressure overshoot in the forward stagnation region because of the viscous effects! Is it right?

Regards,

Chun-Kai

(1). There are only two ways to make sure that a code is working properly. (2).The first one is to refine the mesh step-by-step and plot the surface skin friction coefficient as a function of the mesh size. In this way, you can convince yourself whether you have a converged solution or not. For viscous flow, you must use the surface skin friction coefficient as the convergence parameter. (3). Once you know that the code can give you the converged solution, the next step is to run some test cases. The convergence parameter in this case is still the skin friction coefficient. (4). The pressure distribution can not tell you whether the solution is independent of the mesh used or not. This is because under the same pressure distribution, there exist many possible solutions. (5). For laminar, incompressible flows, there are probably some exact analytical solutions you can use as test cases. (6).Once you have all these exercises done, you can write a paper and submit it for review. You must reveal the methods and formulation used in the code in order for others to give you some advice.

Wowakai,

Creeping flow normally refers to flows where the convection preocess is dominated by the diffusion process. I do not know much about your problem but suspect your aerofoil is not meant to operate in this flow regime. It is, just about, possible that the overshoot is physical but from the plot you sent me at Re=10 the Cp at the stagnation point was 0.7.

Since the effect is local (from the other plot) the most likely culprit is still a numerical problem (not necessarily an error). To repeat my earlier suggestion, high on the list of suspects are: pressure boundary conditions, diffusive flux evaluation on the boundary and pressure smoothing. But it could be something else like a coding slip.

If you want to be certain what is going on then simply evaluate the terms in the transport equation for mechanical energy at your grid points. Plotting the individual terms will show which terms are importatn in transporting the mechanical energy (these have got to be big enough to overcome the dissipation term). The imbalance will also allow you to evaluate your numerical error. It will probably take you an afternoon to perform the exercise but should bring a lot more insight and understanding of the problem. I would be interested in the results so please keep me posted.

regards,

Andy.

Andy,

1)For a N-S flow over a cylinder, it is read from the plot of Fornberg(1980) that

when Re=10 , the Cp/2=0.74 , that is Cp=1.48

where Cp/2=(P-Pinf.)/(ro*U^2) or Cp=(P-Pinf.)/((1/2)*ro*U^2)

2)From the descriptions of Ronald.L.Panton for the Stake flow over a sphere(had been mentioned),it is explained that

"...as Re approaches zero

the viscous diffusion is dominant

and sends VORTICITY far from the body..."

Will it be the VORTICITY(induced far from the body) which may cause action of some work on the local flow?

3)Please review Panton's statement -- "...it reveals that LOW Reynolds number effects cause the forward stagnation pressure on a sphere to become much larger than ideal-flow value of unity."

4)There should be a lot of people, who have done computations of a flow over a cylinder or a sphere. If the pressure overshoot is physical, then it should have be experienced by others. Can anybody talk about his experiences?

5)The disspation function for an incompressible flow is

PHI = mu * (dUi/dXj+dUj/dXi) * (dUj/dXi)

= (1/2) * (dUi/dXj+dUj/dXi)^2

>= 0 always,

but this is the term in the energy equation. In the momentum equations, we get another term(for incomp. flows)

d/dXi ( mu * (dUi/dXj+dUj/dXi) ) = mu * (d2Uj/dXidXi).

The term is possible to cause the pressure overshoot in some special flow field!

Regards,

wowakai

(1). There are four issues which require more study. (2). The accurate prediction of the total pressure field in the turbomachinery applications, which has a great impact on the loss prediction and efficiency calculation. (2). The development of turbulence models which provides physical total pressure distributions. The use of some types of turbulence models has the tendency to produce the total pressure over-shoot which is not acceptable in the turbomachinery applications. By the selection of a proper model, one can avoid this type of non-physical results. (3). As the Reynolds number drops to below Re(O(100)), the viscous diffusion process starts taking over the flow distribution. The proper parameter to use is not the inviscid limit of the total pressure but instead, should be the vorticity distribution. The inviscid limit of the total pressure should not be used in this limit at all. (4). It is always important to make sure that the solution is not a function of the mesh used. In many cases, wrong conclusion was made with inadequate mesh resolution. I hope that the forum is the place to create more interesting problems instead of more awards. CFD can only survive with more unsolved problems.