[sampy]

Hello,
I am trying to setup a case with an axisymmetric injector with periodic boundaries. But I am running into an issue while trying to the assign the periodic condition to a boundary and pair it with its matching boundary. The error/warning I am getting is attached as an image. When I try to the case, it crashes immediately due to periodic boundary matching and duplicate vertices issues. I tried compressing the STL for better tolerances, healing the periodic boundaries, and also increasing the triangles my STL but neighter of these options helped.However, I was able to make the same case work with symmetry boundary conditions but that is not the physics I aiming for. Am I missing something in my case setup?

Thanks,
Sampath
PS: I tried attaching the cvg file of my case setup but it is exceeding cfd-online's attachment size limit.

[angela.wu]

Hello,



It seems like the areas are not matching. One option is to delete one of the periodic boundaries and copy the other face and rotate it. To do this in Studio, go to repair-->delete. Choose selected boundaries as your input method, then select the periodic boundary you want to delete, and click apply. Then go to transform --> rotate, choose the first periodic boundary to rotate. Type the correct rotation angle, and make sure to check number of copies, click apply. This will create a new periodic boundary that is equal to the first periodic boundary. All that is left is to stitch it to your geometry by doing repair--> stitch--> edges. Choose the open edges you want to stitch together.



I hope this was helpful. If you need more help, please contact support@convergecfd.com and we will be glad to take a look at the case setup.


Thanks,


Angela

[sampy]

Hello Angela,
Thank you for the response. Yes, copying the face and stitching with the geometry worked.


I have an additional question. I am trying to simulate injection of a low density gas into a high density one. Irrespective of my best attempts, I am running into "recovering .... because transport equations did not converge or energy extrapolations" issues. I have tried to minimize this issue by adding fixed embedding, AMR, change the solvers to precondition BICGStab and also tried lowering the cfl, cfl_mach, piso tolerances. But none of them work. Any suggestions on how to reduce these convergence issues?
Thanks,
Sampath

[angela.wu]

Hey Sampath,


Can you try the following command in your output directory where there's a converge.log file:
tail -50000f converge.log | grep -e ncyc -e % -e Total -e new -e ABORT -e ERROR -e recover -e limited -e CONVERGE


Please copy what the terminal outputs. We're trying to find what causes the recovery.


Thanks,


Angela

[sampy]

Angela,
Thank you for the prompt response. I attached the log from the command you shared.
-Sampath

[angela.wu]

Can you attach your solver.in and inputs.in?

[sampy]

Sure, I attached the solver.in and inputs.in.
-Sampath

[angela.wu]

A few suggestions: use first-order upwinding and MUSCL flux schemes for momentum, global, and turbulence. Set the flux limiter to minmod. You can also try increasing max # of PISO steps to 20. I would make max_cfl_u 1. Is there a reason why dt_min is 1e-10 and the base mesh is 0.06 mm? What's the overall geometry size?

[sampy]

Thank you, Angela. I will try the suggested settings and will get back to you.


My domain is a few hundred microns in the x,z directions and about 10 mm in y-direction. That's why I used both fixed embedding and amr. My minimum grid size is about 7.5 um. The cell count is close to 10 MM with amr.



One quick question - would the upwinding setting affect the shock structure? I am assuming the sharpness of the shock structures would diminish. Will I be able to recover them once I switch to second order after the flow has stabilized?
Thanks,
Sampath

[angela.wu]

Try MUSCL_CVG as your flux_scheme and reconstructed central difference for the muscl_blend_factors to get a stable flow with less recoveries. Once it's stable, you can change it to muscl_blend_factors to second order upwind. And yes, I would expect the shock to be not well-defined with upwinding, but once you stabilize the flow and switch to second order, it may be better defined.

[sampy]

Hello Angela,


I tried re-running my cases with the suggested changes. I used MUSCL_CVG for the flux schemes with a reconstructed the central difference. This has helped to overcome the energy extrapolation issue. However, my time-steps are still quite low. I realized that cfl_d is pushing the dt to its minimum value. Any recommendations what my cfl_nu should be? It is currently at 5 and I tried lowering it to 2 but that did not help.


Thanks,
Sampath

[angela.wu]

Hey Sampath,


If your timestep is too small and it's limited by cfl_nu, you want to increase it. Try 10 or more and monitor the stability of the flow by looking at recoveries in time.out.



Angela

[sampy]

Thanks, Angela. I should have mentioned in my earlier response that I increased cfl_nu to 20 from the initial value of 5, but that did not help in avoiding the dt_recover. Eventually, i had to lower my cfl_u from 0.75 to 0.3 to keep it stable. It is working fine now.

-Sampath