CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

Verify NS code

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   September 1, 1999, 22:32
Default Verify NS code
  #1
Rothan
Guest
 
Posts: n/a
I had problems in the process of verifying myself-developed 3D NS code to match Blasius. My U/Ue profile is developing much fast in the BL, then the U/Ue curve goes flat and it seems U hits Ue far outside the eta scale. The Re is 10e5 per meter in my calculation and the flat plate is 1. meter long. I set my upper bc as the same of inflow bc (U=Ue,P=Pinf, etc.), and the first y+ of my grid above the flat plate is around 3.0. In BL my grid has 20-30 points which should be enough. Could anyone experienced with Blasius verification give me some advice? Much thanks in advance.
  Reply With Quote

Old   September 1, 1999, 23:49
Default Re: Verify NS code
  #2
John C. Chien
Guest
 
Posts: n/a
(1). There are several areas you can explore. (2). The boundary layer development from a flat plate with sharp leading edge requires the highly stretch mesh in both x and y direction from the leading edge. (3). In this area, you can change the mesh stretching and plot the skin friction distribution. When this is done, try to increase the mesh points until the solution is mesh independent. (4). Then there are two areas which can affect the results. One is the numerical method, and the other is the turbulence model. (5). Normally, a first order method tends to give more diffusive solution. But you can increase the mesh points to reduce the effect. (6). Then the turbulence model is the most troublesome area. There, you can plot the eddy viscosity distribution from the wall to the domain outer boundary. In this way, you can see how the eddy viscosity changes across the boundary layer edge. (7). When I was working on low Re two-equation k-epsilon model in early 70's, I remembered that I needed 100 points to obtain nearly mesh independent solution in a fully developed channel flow. So, 20-30 points is probably not adequate. But then it also depends on the turbulence model you use. (using wall function could reduce the mesh points needed. But then, you still have to show that it is producing mesh independent solution.) (8). You will be surprised that even this seemingly simple problem is actually hard to get it right. So, dont' expect it to match the test results.
  Reply With Quote

Old   September 2, 1999, 02:09
Default Re: Verify NS code
  #3
Zhong Lei
Guest
 
Posts: n/a
I would like to give something in more details.

For such problem, if the Re number is less than 5x10e5, the flow is still laminar and you can compare with the Blasius profile. Usually, 50 grid points are needed within the boundary layer at the location of x=1.0. The first y1 may be taken as less than 1/50 of the boundary thickness, that is to say, y1 < SQRT(x)*0.1/SQRT(RE), where x is the distance from the leading edge. For turbulence computation (Re > 5.0e10e5), 80-120 grid points are needed in the boundary layer, and at least 3 points must be used in the sublayer region ( y+ < 20). The first y+ must be less than 15-20, and may be taken as 5-10. Check the outside boundary in your computation region, and confirm whether yout is large enough, i.e., yout > 5.0/SQRT(Re). Another problem may be the boundary conditions on the outside and the exit. If yout were not large enough and the outside boundary were set to be U=Ue, or the exit condition were set to be du/dx=0, the boundary layer would develop faster.

To verify the grid-independence, a good way is to double the grid number and then compare the velocity and Reynolds stresses profiles.

Z. Lei
  Reply With Quote

Old   September 2, 1999, 09:33
Default Re: Verify NS code
  #4
Janna J.
Guest
 
Posts: n/a
thanx for sharing.
  Reply With Quote

Old   September 2, 1999, 10:24
Default Thanks
  #5
Rothan
Guest
 
Posts: n/a
I am grateful for your prompt and detailed advice.
  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
The FOAM Documentation Project - SHUT-DOWN holger_marschall OpenFOAM 242 March 7, 2013 13:30
Open Source Vs Commercial Software MechE OpenFOAM 28 May 16, 2011 11:02
Design Integration with CFD? John C. Chien Main CFD Forum 19 May 17, 2001 15:56
own Code vs. commercial code Bernhard Mueck Main CFD Forum 10 February 16, 2000 11:07
public CFD Code development Heinz Wilkening Main CFD Forum 38 March 5, 1999 12:44


All times are GMT -4. The time now is 04:26.