Problem results

Questions and remarks about code_saturne usage
Forum rules
Please read the forum usage recommendations before posting.
Loïc A.
Posts: 9
Joined: Mon Mar 10, 2014 7:56 pm

Problem results

Post by Loïc A. »

Hello,

I'm using Code_Saturne version 3.0.3.

Currently, I'm trying to simulate the flow on a fat plane. I chose a rectangular domain (2D). The definition of the geometry consists of two joint blocks (using face joinning).
I put a wall condition to the bottom wall, symmetries conditions to the side walls, an inlet and an outlet condition to the extremities. I also wrote the following code for the upper face of the domain:

Code: Select all

call getfbr ('Farfield',nlelt,lstelt)
!==========
do ilelt = 1,nlelt

  ifac = lstelt(ilelt)
  iel = ifabor(ifac) !cell adjacent to boundary face
 
   itypfb(ifac) = iparoi

    icodcl(ifac,iv) = 1
    icodcl(ifac,iu) = 3
    icodcl(ifac,iw) = 1

    icodcl(ifac,ik) = 1
    icodcl(ifac,iomg) = 1
   

    rcodcl(ifac,iv,1) = 0.d0                           
    rcodcl(ifac,iu,3) = 0.d0
    rcodcl(ifac,iw,1) = 0.d0

    rcodcl(ifac,ik,1) = 0.000833d0 
    rcodcl(ifac,iomg,1) = 0.1318d0

enddo

My simulation run but the results are not good and I don't understand why.

I join a pdf with the graphic of the evoluation of the Cp (Coefficient of pressure) on the upper wall and the graphic with the inlet profil and the oulet profil. We see that the flow has not accelerated between the inlet and the outlet of the domain. The conservation law is not respected. Normally due to the development of boundary layer on the wall, the flow will have to accelerate but it's not the case here.

Anyone has an idea about what's wrong with the simulation? I put my .xlm file and my mesh file if someone wants to test it.

Thanks in advance for your help.

Best regards,
Loïc.
Attachments
Simulation2D.rar
(713.85 KiB) Downloaded 94 times
Brian Angel
Posts: 98
Joined: Mon Jul 22, 2013 12:53 pm

Re: Problem results

Post by Brian Angel »

Hello Loic,

I will take a look at this case but can you please clarify what you are trying to achieve with the wall boundary condition on the top of your flow domain that which has been coded in the user routine). Can you also let me know for how many iterations you have run this simulation.

Regards,

Brian Angel.
Loïc A.
Posts: 9
Joined: Mon Mar 10, 2014 7:56 pm

Re: Problem results

Post by Loïc A. »

Hello Brian,

Thank you very much for your reply.

The surface on the top of the flow must be considered as an ideal upper boundary, wall specified shear equaling zero (=zero-vorticity). That's why I chose to impose the u-velocity gradient to zero and the other components of the velocity to zero.

For this case, I take 300 iterations. I just tested with a larger number of iterations, the evolution of the Cp is improved to the extent that decreases in the direction of flow. But there is almost no acceleration.

I hope my answer is sufficiently understandable (my English isn't perfect, my apologies about that).

Thanks again for your help.

Best regards,
Loïc.
Brian Angel
Posts: 98
Joined: Mon Jul 22, 2013 12:53 pm

Re: Problem results

Post by Brian Angel »

Hello Loic,

If you haven't already done so, can you try to run this case for 3000 iterations and let me know what results you get.

Best regards,

Brian Angel.
Loïc A.
Posts: 9
Joined: Mon Mar 10, 2014 7:56 pm

Re: Problem results

Post by Loïc A. »

Hello Brian,

I run it for 5000 iterations but the problem is still present. I check the balance of conservation of mass and momentum. It appears that suction occurs on the upper face. This explains that the flow doesn't accelerate.

The mistake must therefore come from the implementation of the boundary condition on the upper face. But I can't find it.

Best regards,
Loïc.
Brian Angel
Posts: 98
Joined: Mon Jul 22, 2013 12:53 pm

Re: Problem results

Post by Brian Angel »

Hello Loic,

I have run your case using CS v3.2.1 and have, I believe, the same result that you have. So, I ran the case setting the condition "Farfield" as a wall boundary in the GUI with no user coding. The results after 2000 iterations look reasonable with an acceleration of the air in the duct. I then added in your user routine but with no coding, CS simply calls the user routine but does nothing else. Again the results look reasonable. I then added your user coding except for the ICODCL for the velocity components. Again the results look reasonable. It is only when the ICODCL is added that the results go back to what you have. With the setting for ICODCL(ifac,iu)=3 are you sure that this is going to give you what you are looking for?

Also, what do you mean by "an ideal upper boundary"? What are you looking to achieve with such an ideal boundary?

Best regards,

Brian Angel.
Loïc A.
Posts: 9
Joined: Mon Mar 10, 2014 7:56 pm

Re: Problem results

Post by Loïc A. »

Hello Brian,

Infact, I wish that my upper limit does not affect the flow that occurs on the lower solid wall. This is like placing the upper wall to infinity. In order to achieve this, I impose a sliding wall.

I had initially put the component u of the velocity equal to the inlet velocity (1m/s) and the other to zero. But the results do not match the condition that I want to impose. I get a "connection" at the speed of 1 m / s on the upper side (see velocity profiles in pdf file). However in this case, we see the acceleration and the inlet mass flow is well equal to oulet mass flow.



I then chosen to set the wall shear stress equal to zero: . That is why I set the gradient of the component of velocity equal to 0.

(Outside the boundary layer, it's a perfect fluid flow wich is irrotational. Then the idea is to impose a zero-vorticity condition: (2D) with v=0).


Don't hesitate to tell me if my answer is not clear. If you want to see it, the velocity profiles obtained from fluent, therefore I would like to reproduce on Saturne, are in the pdf file.

Thank you very much for your help anyway.

Best regards,
Loïc.
Attachments
Code_Saturne_Forum.pdf
(338.9 KiB) Downloaded 106 times
Brian Angel
Posts: 98
Joined: Mon Jul 22, 2013 12:53 pm

Re: Problem results

Post by Brian Angel »

Hello Loic,

Essentially you want a slip wall condition on the upper Farfield boundary with du/dy=0 but v = w = 0 assuming that the flow is essentially 1D in the vicinity of this upper boundary. I'll have a look and come back to you.

Best regards,

Brian Angel.
Loïc A.
Posts: 9
Joined: Mon Mar 10, 2014 7:56 pm

Re: Problem results

Post by Loïc A. »

Hello Brian,

Yes, it's exactly this condition that I want to impose.

Best regards,
Loïc.
Jacques Fontaine
Posts: 118
Joined: Mon Feb 20, 2012 2:07 pm

Re: Problem results

Post by Jacques Fontaine »

Hello,

Why you did not use a symmetry condition on the upper wall ?
Regards,
Post Reply