Simulation only Converges with Slip Boundary Condition

Using SimScale Fluid Flow / CFD
1

I am running a turbulent steady state simulation of fluid flow through a unit cell placed in a bounding box. (Here is the project: https://www.simscale.com/workbench/?pid=2384453580176520466). I am having trouble with my boundary conditions and reaching convergence.

I have a velocity inlet condition and a pressure outlet condition (gauge pressure = 0). On the other 4 walls of the bounding box, I have a free slip condition. On the unit cell itself, I have tried both free slip and no slip conditions, but I can only reach convergence on the free slip condition. I also tried inflating the boundary layer on the faces of the unit cell and using no-slip, but this did not converge either.

Is it physically meaningful to use free slip on the unit cell? If not, how can I reach convergence using no-slip on the unit cell?

1 Like
2

Hi, this is Fillia :slight_smile:I just checked your latest run, and it seems there is steadiness in the residual control results.
Regarding the omega, you can try reducing the absolute tolerance to 1e-8, this could solve the oscillation issue:

omega
omega992×894 95 KB

To improve convergence, there are a few things that you can do:

  1. If you are using full resolution wall treatment make sure you have generated an appropriate boundary layer, that provides a y+<1. Have a look here: How to Control and Analyze Y+ in Meshing Simulation | SimScale
  2. Increase the domain. Use Figure 4. from this tutorial as a rule of thumb.
  3. Add a couple of region refinements, as you can see in the golf ball tutorial I sent you above.

Lastly, the No-slip wall condition is indeed the correct choice for the unit.

Best regards,
Fillia

1 Like
3

@tsite Thank you very much for the response. I am working on implementing your suggestions.

Regarding the boundary layer thickness, the y+ values are shown for a the mesh generated with the default boundary layer settings. The max y+ value is only 0.158 (see picture below), so I think using full resolution on the walls of the unit should work.

I will try another simulation with the proper domain size, again verifying y+<1, with a couple of regional refinements and will update you in this thread!

y+
y+1440×1080 116 KB

1 Like
4

@tsite Using the configuration suggested in the golf ball tutorial, I was unable to incorporate regional refinements without having a “mesh failure” message. The error message says that the machine ran out of memory, so I am guessing that the regional refinements I created were too fine.

I implemented all other parameters you suggested, and the performance has improved dramatically, but still is not converging for pressure. The residuals are shown here: (https://www.simscale.com/workbench/?pid=2384453580176520466&rru=0a057f2c-230b-426d-9046-009667312ab9&ci=0c201768-b5d5-4f71-a01b-0a2cdb6c0300&ct=CONVERGENCE_PLOT&mt=SIMULATION_RESULT).

Do you have any suggestions now that only pressure is not converging? Is the regional refinement necessary, perhaps? And if so, how can I implement the regional refinement since the message I am receiving is suggesting the refinement requires too great of a computational load?
Thanks again!

5

@tsite

I went back to double check, and I had y+<1 satisfied near the unit, even without regional refinements in the mesh. Could it still be possible that regional refinements are causing the non-convergence, or do you think it is stemming elsewhere?

newewst run y+
newewst run y+1440×1080 123 KB

6

Hey, actually the convergence doesn’t seem that bad, try the following things:

  1. Switch to ‘Fixed value’ instead of ‘Mean value’ for your Pressure outlet bc.
  2. Increase the absolute tolerance of the omega to 1e-8 from 1e-6
    These will reduce the oscillation. Moreover , you can work on your mesh by adding region refinements, using the cartesian boxes you have already created. They don’t have to be really fine, a maximum element size of 0.0005-0.0001 would work for them.