[kahjoonyong]

Hello everyone,

I am trying to simulate an autoignited Cabra flame. The flame setup is according to the following paper. http://docdro.id/oVxNyER

I first tried to reenact the case with RANS and was somewhat successful. However when I tried to do the exact same case with LES the results were not at all accurate. Here is the images of the results I got. https://imgur.com/a/zRWjL. The LES results I got do not have the turbulent flow (dissipative flamelets or Eddies) at the flame boundary at all.

I tried to use different LES models : Smagorinsky, Dynamic Smag, Dynamic Structure. All of them gave me the same result. I even manipulated the velocity fluctuation at the inlet boundary and the turbulence model constants. It seemed to me that the viscosity of the flow was too low or the mixing was bad. Can anyone shed a light into this?

Case Setup file (Converge v2.3): Attachment

Thank you very much.

Kah Joon Yong

[Blanco]

Hi,

I'm not an expert of LES, but have you tried to change the AMR settings? I've seen you're using the default subgrid values for velocity and temperature, maybe they are not the best option for you case. Moreover, you're limiting the maximum cell number to 2e6, did you reached that value in your sim?

[ksrivast]

Hello Kah Joon,

It looks like the paper was using a LES mesh with grid sizes of 0.37mm (with thickening). Currently, with the AMR settings in your case setup, you can only go down to 0.5mm (and 1mm in the z direction since you have an anisotropic grid). Could you try increasing your AMR embed scale/grid settings so as to match them with that of the paper?

Also, Blanco offers a valid point. Please check to see if you are actually reaching the maximum level of refinement you have in your AMR settings. If not, decrease the value for sub-grid criterion. Also, increase your maximum cell count to ensure you have enough cells available for AMR.

I would also recommend having a fixed embedding (equal to the maximum level of refinement you desire) right at your jet inflow. This can either be a shape embedding or a boundary embedding. This will help seed the AMR and make it more effective.

Hope this helps.

Sincerely,

Srivastava

[kahjoonyong]

Thanks for all your replies. Those suggestions are actually valid points! Before you guys replied just yesterday evening I just thought about that as well. I am allowing the simulation to run now by increasing the embedding scale. The maximum number of cells were not reached instead it increased at the beginning and then decreased to around 200k cells. I assumed that the cell size was not fine enough. After increasing the embedding scale to 6 AMR generated about 1.5 million cells currently and the simulation became significantly slower. I am not sure if I should decrease the SGS value or increase the embedding scale. I will try out both.

Again thank you very much for the suggestion.

[williamchina]

Hi,

I am also simulating Cabra Flame, but instead using the TPDF method in Ansys Fluent. However, I would also like to try AMR using Converge. The major concern is that how good the result will be. Do you have any paper on the results for now?

Best,
Weiqi

[kahjoonyong]

I am still trying to get the result to match the one from the paper I've mentioned. So far I am facing a problem in computing power to make AMR works for LES. It seems like the grid size controls the shape of the jet and flame as well as the jet penetration. I am having a base grid size of 0.008x0.008x0.008 with a Tsgs=1K and vsgs=0.1m/s both with scale of 6. Still the jet penetrates to far and no mixing is captured after a few milliseconds. I tried to decrease Tsgs and Vsgs as well as increase the Scale, but the cell count skyrockets (exceeds 5mil cells) and my small 16 core cluster computer cannot handle that I am still trying to figure out a way to improve it.

[williamchina]

What's the problem with the cell counts? If you have a parallized cluster, will the cells be distributed on different nodes? (not processors). How many nodes(cpus) you are using?
BTW, do you have any problems with the time step size? When you use refined grid, you probaly have to use a very small time step, do you?

[kahjoonyong]

There is a limitation here in my university for students to access the cluster. I could only send my simulation to one node each time. And our strongest node has only 16 core (instead of 16GB, what was I thinking!), the others have 8 cores. Furthermore, I have discussed with my adviser, he said the the calculation speed could be limited by the communication between 2 nodes.

Regarding time step, I am using variable timestep which is limited by CFL numbers in CONVERGE. For the LES simulation the time step goes down to around 3e-6s.

[ksrivast]

Hello Kah Joon,

If you still have excessive penetration and lack of mixing, it can help to have a closer look at the fluctuations you're adding on the inflow. We have found that to get the correct jet development for gaseous jets, we need to add fluctuations to the inflow, otherwise the jet development is too slow. The old case setup you had shared earlier did have fluctuations enabled. I would suggest adding fluctuations in all directions. Also, it would be good to investigate how sensitive your results are to fluctuating intensity and fluctuation length scale.

Also, I hope you're not relying only on AMR for resolution. Please provide a permanent fixed embedding (conical) covering the initial volume of jet development. (Similar to how we provide nozzle embedding (fixed) for our case that include spray models)

Hope this helps. Please let me know of the results.

Sincerely,

Srivastava

[kahjoonyong]

Hello Srivastava,

thank you for your suggestion. I have tried including a conical fixed embedding region for the mesh refinement. However, the results wasn't improved. On the other hand, that alone added 1-2 million cells to the calculations. That made me wonder if that fixed embedding is necessary at all. I would take your suggestion and try again.

Regarding the fluctuation, I have not manipulated the length scale and the intensity. This is because it was mentioned in the paper that the velocity fluctuation prescribed at the jet flow has an intensity of 0.0005 and the jet flow was 'a fully developed turbulent pipe flow' which translate to a length scale of about 0.038*D_jet. It wasn't mentioned that the Coflow has any fluctuation therefore I do not prescribed that.

Could you elaborate on how to prescribe fluctuation in all directions?

Thank you very much, your reply gave me a good insight on this matter. However each calculation takes a long time and I could hardly manipulate each variable to test it out as quick as possible.

Sicerely

Kah Joon

[ksrivast]

Hello Kah Joon,

Fixed embedding would help "seed" the AMR. Better capture of the gradients through fixed embedding can help it develop and grow more effectively and thus provide more accuracy. To conserve on cell count due to fixed embedding, try smaller volumes for your conical region. A small spherical embedding at the inlet of the jet could be considered as well.

To prescribe fluctuations in all directions, change the last entry of the parameter inflow_fluctuating from 0 to 1 in boundary.in for your fluctuating inflow boundary. This can also be done in STUDIO, under the Boundary tab, by changing Direction from Normal to All, for your fluctuating inflow boundaries.


Sincerely,


Srivastava

[kahjoonyong]

Hello Srivastava,

I currently have a prescribed Fixed Embedding as a boundary embedding for the Jet Inflow instead of a cylinder.

I am using Converge v2.3 and it seems like there is no extra entry for the parameter inflow fluctuating other than intensity, length scale. There is also no option to choose the Direction of the fluctuation in STUDIO. Is this feature enabled in v2.3 and I need to activate it manually somehow?

Sincerely,
Kah Joon

[ksrivast]

Hello Kah Joon,

If your fixed embedding is boundary embedding, do make sure you have enough embed layers. Just one or two is not enough. What version of v2.3 CONVERGE solver are you using? What's the release date for your CONVERGE STUDIO v2.3 (check the top of your message log)?

Earlier, for inflow_fluctuating BC we only added fluctuations to the velocity component normal to the boundary. This is because for wall-bounded flows like channel flow, having non-zero velocity in the tangential direction in cells close to wall leads to unphysical oscillations. However for cases without walls such as turbulent jet, the velocity fluctuations must be added to all 3 components to get the mixing correct.


Sincerely,

Srivastava

[kahjoonyong]

* This software is Proprietary to Convergent Science Inc. (2008) *
* CONVERGE Release Build 2.3.16 *
* Sep 06, 2016

I have included 3 layers. I am not sure if this is enough. I have not compared it with the other settings as I was testing the scale and the subgrid criterium of AMR and each calculation for an increased scale takes a long time.

Is there a way to add the inflow fluctuating to all directions for this version of Converge? Or should I create a modified geometry with an extrusion for the jet?

[ksrivast]

Hello Kah Joon,

Try this syntax : inflow_fluctuating 0.05 0.03 1

We recommended you download our latest version of STUDIO to have this selection in your GUI. We also recommend you use our latest version for CONVERGE v2.3.

Sincerely,

Srivastava

[kahjoonyong]

Hello Srivastava,

Thanks for your suggestion. I will reflect this to the admins in my university. This version of Converge is installed in my university's Linux computer and I have no admins right to modify it. To update a version is also not something simple which I can do. I appreciate your help wholeheartedly. I will try out the syntax for the time being.

Just to be clear. I should overwrite this syntax for the inflow_fluctuating parameter in boundary.in file, am I right?

Currently in boundary.in :

#-----------------------------------------------
2 Jet
inflow_fluctuating 0.0005 0.000174
velocity Dirichlet 0.0 0.0 100.0
pressure Neumann 0.0
...

replace with

#-----------------------------------------------
2 Jet
inflow_fluctuating 0.0005 0.000174 1
velocity Dirichlet 0.0 0.0 100.0
pressure Neumann 0.0
...

sincerely
Kah Joon Yong

[ksrivast]

Yes. Hope it helps.

Sincerely,

[kahjoonyong]

Thank you very much. I am simulating it now.

[dricehack]

Originally Posted by ksrivast

Hello Kah Joon,

If you still have excessive penetration and lack of mixing, it can help to have a closer look at the fluctuations you're adding on the inflow. We have found that to get the correct jet development for gaseous jets, we need to add fluctuations to the inflow, otherwise the jet development is too slow. The old case setup you had shared earlier did have fluctuations enabled. I would suggest adding fluctuations in all directions. Also, it would be good to investigate how sensitive your results are to fluctuating intensity and fluctuation length scale.

Also, I hope you're not relying only on AMR for resolution. Please provide a permanent fixed embedding (conical) covering the initial volume of jet development. (Similar to how we provide nozzle embedding (fixed) for our case that include spray models)

Hope this helps. Please let me know of the results.

Sincerely,

Srivastava

Hi Srivastava

Could you please elaborate on adding fluctuations to the inlet boundary on proper jet development? Perhaps, any links to papers.

Thanks