[GaryPei]

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

[fluid23]

how are you simulating this? RANS, LES, DNS? You haven't given enough context for people to be able to help you.

[GaryPei]

Originally Posted by fluid23

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?

[fluid23]

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]

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

[LuckyTran]

I don't know anything about the "success" others have had with this simulation but... there is a contraction between:

Originally Posted by GaryPei

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

Originally Posted by GaryPei

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]

Thank you for your time

[GaryPei]

Originally Posted by LuckyTran

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!

[LuckyTran]

Originally Posted by GaryPei

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.

[GaryPei]

Originally Posted by LuckyTran

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.

[LuckyTran]

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.