CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > Siemens > STAR-CCM+

Validation of the flow over flat plate

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

Like Tree4Likes
  • 1 Post By fluid23
  • 1 Post By fluid23
  • 1 Post By LuckyTran
  • 1 Post By LuckyTran

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 23, 2019, 17:50
Default Validation of the flow over flat plate
  #1
New Member
 
gen pei
Join Date: Aug 2019
Posts: 6
Rep Power: 2
GaryPei is on a distinguished road
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 no-slip wall and the top as no-slip 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
Attached Images
File Type: jpg Mesh.jpg (88.7 KB, 15 views)
File Type: png Streamwise velocity.png (9.3 KB, 14 views)
File Type: jpg WSS.jpg (30.3 KB, 15 views)
File Type: jpg BL thickness.jpg (20.0 KB, 13 views)
GaryPei is offline   Reply With Quote

Old   October 24, 2019, 16:02
Default
  #2
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 776
Rep Power: 12
fluid23 is on a distinguished road
how are you simulating this? RANS, LES, DNS? You haven't given enough context for people to be able to help you.
GaryPei likes this.
fluid23 is offline   Reply With Quote

Old   October 24, 2019, 16:47
Default
  #3
New Member
 
gen pei
Join Date: Aug 2019
Posts: 6
Rep Power: 2
GaryPei is on a distinguished road
Quote:
Originally Posted by fluid23 View Post
how are you simulating this? RANS, LES, DNS? You haven't given enough context for people to be able to help you.
Thanks a lot for your response.

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?
GaryPei is offline   Reply With Quote

Old   October 24, 2019, 17:45
Default
  #4
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 776
Rep Power: 12
fluid23 is on a distinguished road
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.
GaryPei likes this.
fluid23 is offline   Reply With Quote

Old   October 27, 2019, 02:51
Default
  #5
New Member
 
gen pei
Join Date: Aug 2019
Posts: 6
Rep Power: 2
GaryPei is on a distinguished road
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
GaryPei is offline   Reply With Quote

Old   October 27, 2019, 21:17
Default
  #6
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,567
Rep Power: 44
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
I don't know anything about the "success" others have had with this simulation but... there is a contraction between:
Quote:
Originally Posted by GaryPei View Post

I am trying to simulate a simplest case of zero pressure flow over flat plate (2D, laminar, incompressible) and observe the laminar boundary layer.
and
Quote:
Originally Posted by GaryPei View Post

I set the inlet and outlet as internal periodic interfaces, the bottom as no-slip wall and the top as no-slip wall with 0.2 m/s tangential velocity (freestream velocity). Also I set the initial velocity as 0.2 m/s.
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?
GaryPei likes this.
LuckyTran is offline   Reply With Quote

Old   October 27, 2019, 21:32
Default
  #7
New Member
 
gen pei
Join Date: Aug 2019
Posts: 6
Rep Power: 2
GaryPei is on a distinguished road
Thank you for your time
GaryPei is offline   Reply With Quote

Old   October 27, 2019, 21:34
Default
  #8
New Member
 
gen pei
Join Date: Aug 2019
Posts: 6
Rep Power: 2
GaryPei is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
I don't know anything about the "success" others have had with this simulation but... there is a contraction between:

and

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?
Thank you so much for your reply!

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!
GaryPei is offline   Reply With Quote

Old   October 30, 2019, 12:41
Default
  #9
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,567
Rep Power: 44
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Quote:
Originally Posted by GaryPei View Post
Thank you so much for your reply!

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!
This is nothing to do with cost, it's about problem definition.

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.
cwl likes this.
LuckyTran is offline   Reply With Quote

Old   November 1, 2019, 12:41
Default
  #10
New Member
 
gen pei
Join Date: Aug 2019
Posts: 6
Rep Power: 2
GaryPei is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
This is nothing to do with cost, it's about problem definition.

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.
Thank you for your answer. I apologize for my lack of fundamental knowledge for the fluid.

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 wall-normal 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.
GaryPei is offline   Reply With Quote

Old   November 4, 2019, 15:52
Default
  #11
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,567
Rep Power: 44
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Are you referring to the recycled-rescaling 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 Star-CCM. 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 Star-CCM. 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 Cd-Adapco folks will be very happy to see you do it.
LuckyTran is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 08:51.