Couette flow in fluent
 

I am trying to analyse couette flow in fluent. Couette flow is basically flow fluid between two parallel plates in which one plate is moving. Due to the motion of one plate the motion is imparted to the fluid.
I am analysing in 2D. I have created rectangle. I am considering the top plate as moving with velocity of 1m/s. So, what should be my boundary conditions to left side, right side, top plate and bottom plate?

The "bottom" boundary should be a wall with zero (or -1 m/s, that is up to you) tangential velocity.
"Left" and "right" boundaries should be connected through a periodic boundary condition.

BTW: the description of this sub-forum clearly states "do not post fluent questions here"

Thanks flotus1 for your reply. Further I would like to know for the periodic boundary condition how should I compute the offset. Should I let be computed automatically by fluent. I actually do not understand this concept of offset.

PS:Sorry for posting question in this forum. Can you also tell how can I transfer this question the software/fluent forum.?

The offset is the vector from one boundary in the periodic pair to the other boundary.
Lets assume your domain for Couette flow has an extent of 1m in x-direction, then the offset vector would be (1,0)m.

Usually fluent computes the vector correctly, but you should check it again.
If Fluent for whatever reason does not compute the vector correctly, you can input it manually.

Moving the post is not possible for you, only moderators can do that.
I just wanted to let you know because there are tons of questions related to fluent in this forum.

I applied the periodic boundary condition. But I am confused about the exact method. Is it necessary to match the periodic edges in meshing?
I get a message cannot create surface from sliding interface zone, creating empty surface.

As far as I know, the error message you get is not related to periodic boundaries.
Did you follow the steps outlined in the tutorial "Modeling Periodic Flow and Heat Transfer"?

As far as the meshing is concerned, it is not necessary to set up periodicity here. You can do it in fluent, following the steps described in the tutorial.
Of course you need to make sure that the topologies of the two faces you want to make periodic are identical.
And the meshes on both faces (lines in your case, since you are dealing with 2D) should be identical. Otherwise the periodic boundary condition will rather be an interface that needs lots of interpolation.

I followed all the steps given in the tutorial of modeling periodic flow and heat transfer. My edges are totally identical. Now i don't get the error. however, solution does not converge. The residuals oscillate and then flatten out. What could be the reason?

Post a figure of the residuals.

first, check the steady solution for small Re number, check also to have a divergence-free velocity field

Well, after numerous tries I did not get convergence.

This is the image of my residuals:
https://imageshack.com/i/hlb214dfj

Filippo might be on the right track here.
What is the Reynolds number in your simulation? Are you sure it is low enough for steady laminar flow?

Oh, yes I overlooked that aspect. The reynolds number in my case is around 1x10^6. So, I think it must be a turbulent flow. I am actually following tutorial by Penn State University where they haven't turned the turbulent models.

Also, I observed the following:
Whenever I use second order upwind for discretisation of momentum I get the case of no convergence and flat residuals. However, with first order upwind I get convergence. The velocity profile is fairly unaffected though.

I have plotted my velocity plot on a centerline in my domain. Is it according to the expectations?
https://imageshack.com/i/ex8c56afj

Pointless to discuss the results of spatially under-resolved two-dimensional DNS solved with a steady state solver.

So, what could be the problem? Is it the periodic boundary condition that is creating a problem?

The problem is the Reynolds number.
At least to my understanding, Couette flow implies laminar flow.

The flow you are modeling is turbulent. From the residuals you posted I could derive that you are not using any turbulence model.
You can either lower the Reynolds number or use some proper turbulence modeling.
The latter would require a finer mesh in wall-normal direction, 10 cells are definitely too few to get yplus values in the correct range.

I reduced the Reynolds number to 5000 by reducing the velocity of the moving wall i.e. the top plate. However, I havent got any convergence. Residuals oscillate but their average behaviour is flat.

you should set Re=1

http://www.mne.psu.edu/cimbala/Learn...uette_flow.pdf

http://www.mne.psu.edu/cimbala/Learn...uette_heat.pdf

i don't know you may find these ones but you can use these pdf's for your solutions

Yes Ali, I am following the same one. My dimensions and all specifications are the same as in the tutorial. However, I am having certain issues about convergence which I am currently trying to sort out.

convergence problem is limited for a specific parameter or all parameters are non-convergent? if continuity is the problem you can fix pressure relaxiation value from= solve>controls>solution. you may use for other parameters but i'm not sure if it helps cause i never tried them :)