
[Sponsors] 
Validation of the flow over flat plate 

LinkBack  Thread Tools  Search this Thread  Display Modes 
October 23, 2019, 17:50 
Validation of the flow over flat plate

#1 
New Member
gen pei
Join Date: Aug 2019
Posts: 6
Rep Power: 2 
Dear Experts,
I am trying to simulate a simplest case of zero pressure flow over flat plate (2D, laminar, incompressible) and observe the laminar boundary layer. I set the inlet and outlet as internal periodic interfaces, the bottom as noslip wall and the top as noslip wall with 0.2 m/s tangential velocity (freestream velocity). Also I set the initial velocity as 0.2 m/s. The domain is 8 cm long by 6 cm high. I used polygonal mesh with y+=0.1 for the closed grid point to the bottom wall, which is 0.0001 m cell size. The surface grow rate is 1.01. Please attached Mesh figure. I ran the simulation for solution time of 5 s with mean CFL=0.8. Attached Streamwise Velocity figure shows the velocity field. However, when I compared the simulation result to the Blasius solution: Boundary layer thickness= 4.91 * length* Re_x^(1/2); The simulated boundary layer thickness at 0.99 U (3.5 cm) is about 20% lower than the Blasius (4.3 cm) (see the attached BL thisckness figure). Also the wall shear stress is higher (see attahced WSS profile). While previous CFD studies in literature often yield a great agreement. I also tried other tests with a finer mesh (y+=0.05) or 3D case or larger iteration numbers, while they all gave the same results. I really have no idea why it happened and what I should do next. Thank you so much for reading it through. It would be EXTREMELY helpful if you can help me find any issues in my simulation or give me any advice! Please let me know if I can provide more information. Thank you! Regards, Gary 

October 24, 2019, 16:02 

#2 
Senior Member
Matt
Join Date: Aug 2014
Posts: 776
Rep Power: 12 
how are you simulating this? RANS, LES, DNS? You haven't given enough context for people to be able to help you.


October 24, 2019, 16:47 

#3  
New Member
gen pei
Join Date: Aug 2019
Posts: 6
Rep Power: 2 
Quote:
It is my first post and sorry that I did not make it clear. I used the DNS and no turbulent model was selected (only Laminar model). Would you please give me any advice to check my simulation? 

October 24, 2019, 17:45 

#4 
Senior Member
Matt
Join Date: Aug 2014
Posts: 776
Rep Power: 12 
I will have to defer to someone with more expertise with DNS, but be advised that wall y+ is usually discussed in terms of a turbulence model. It still has a physical significance in laminar flow, but you are not likely to find wall y+ recommendations for a laminar DNS solution. Normally, the goal with DNS is to resolve all of the Kolmogorov scales. There are various ways to approach this. A quick google search will yield lots of helpful information.


October 27, 2019, 02:51 

#5 
New Member
gen pei
Join Date: Aug 2019
Posts: 6
Rep Power: 2 
Thank you for your advice!
I still have no idea how to refine my model. Once I solve this issue I will post the solution here 

October 27, 2019, 21:17 

#6  
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,567
Rep Power: 44 
I don't know anything about the "success" others have had with this simulation but... there is a contraction between:
Quote:
If you use periodic BC's and a top moving wall, this is no longer the flow over a flat plat which should follow the Blasius solution. It's flow between parallel plates, which is a Couette flow. The velocity profile is linear and there is no concept of boundary layer thickness (the boundary layer occupies the entire region between the plates). What's going on here? 

October 27, 2019, 21:32 

#7 
New Member
gen pei
Join Date: Aug 2019
Posts: 6
Rep Power: 2 
Thank you for your time


October 27, 2019, 21:34 

#8  
New Member
gen pei
Join Date: Aug 2019
Posts: 6
Rep Power: 2 
Quote:
It is a great point and I think it is worth to try other BC conditions. But The thing is I need to keep the periodic BC's to reduce the cost so I cannot set the inlet condition as inlet velocity to define the freestream velocity (that's why I set the moving wall and initial velocity). Would you please give me any advice about setting the BC's for flow over flat plate? Thank you! 

October 30, 2019, 12:41 

#9  
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,567
Rep Power: 44 
Quote:
If you use periodic BC's, the solution you should be trying to match is the solution for Couette flow (which is a simple linear profile). You'll never get Blasius solution. In fact, if you match the Blasius solution, that would just plain be wrong. You must use an inlet velocity for it to be flow over a flat plat. You don't get to argue about this unless you reprint all the introductory fluid mechanics books printed in this century. The community has already decided to name it so. I advise you to stop calling it flow over a flat plate, because that's not what you're simulating. If you want to simulate flow over a flat plat, then use the right BC's. 

November 1, 2019, 12:41 

#10  
New Member
gen pei
Join Date: Aug 2019
Posts: 6
Rep Power: 2 
Quote:
After I read your reply, I reviewed more literature and you are absolutely correct. My BC's are set wrong and the normal periodic BC's should not be applied for flow over flat plate due to the heterogeneous streamwise flow. Alternatively, the previous study usually applied the modified periodic BC's. There are two modified BC's are actively used. One is proposed by Spalart (1998). This method defines a new coordinate replaced the wallnormal coordinate along which the BL is assumed constant in streamwise direction. The NS equations are transformed into this coordinate system, which introduces a new term to the equations. Another method is a simplified version of the Spalart method by Lund et al. (1998). This method extracts the velocity field from a plane near the domain exit and rescales it using the Spalart idea, and then reintroduce it as a boundary condition at the inlet. I am trying to get more fundamental knowledge and figure out how to apply these methods in the Starccm+. I am just wondering if you have any related experience and would you please give me any advice of setting these methods in Starccm+? Thank you. 

November 4, 2019, 15:52 

#11 
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,567
Rep Power: 44 
Are you referring to the recycledrescaling method for generating turbulent inflow data for LES and DNS? That approach is for turbulent boundary layers... I worked closely with a colleague who did this in OpenFOAM. It should be anyway be very doable in StarCCM. If your case is laminar, then it's even simpler.
Periodic BC is not the way to go. You extract the velocity at the outlet and remap it onto the inlet (and also introduce some functions to rescale it before remapping it). This approach is much more akin to the mapped interface and hence why we don't like to call it periodic. Definitely look into the data mapper tool in StarCCM. You'll still have to figure out some custom field functions and define some intermediate/auxiliary functions to rescale the BL. I wonder if you can maybe even find this already done by someone else or on the Steve Portal. It is a prerequisite for doing DNS and I imagine a few people might have attempted it. If not, the CdAdapco folks will be very happy to see you do it. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
problem in Cf in flow over flat plate  mb.pejvak  Main CFD Forum  13  December 2, 2013 01:13 
Low Reynolds Number Flow over a Flat Plate  Go  FLUENT  4  August 28, 2013 06:19 
Simulations Flow 3D over Flat plate  baoaero  OpenFOAM  7  June 7, 2013 06:53 
supersonic flow over flat plate  varunjain89  Main CFD Forum  1  March 23, 2010 09:26 
Turbulent Flat Plate Validation Case  Jonas Larsson  Main CFD Forum  0  April 2, 2004 11:25 