[joaofl]

Thats true. I got that from the paper. Trying this right now!

Thanks again.

[joaofl]

By the way, do you think RAS is a better approach?

[ni-openfoam-user]

It all depends on what you're trying to achieve and what you're interested in.

In LES: the larger 3D unsteady turbulent motions are directly solved. The effect of the smaller scale motions are modelled.

In RANS: The model solves the transport equations for the mean flow quantities only and all the scales of turbulence are modelled.

To help please see the attachments below: the second shows a direct comparison between RANS and LES results using FLUENT.

Hope it helps,

James

[joaofl]

Great plots. This leaves no doubts about my choice. LES might produce the results I expect. The main issue is with my setup.

I made the nozzle conic, with a radius in the end to avoid the effect of sharp edges, and add extra volume to it, to create a higher pressure area, for the jet to occur. Used ur formula to calculate k.

But now, the simulation crashes at t=0.145 (the pressure distribution at the last time instant is the attached snapshot)

Do you have any clue why it happens? Should I chose another pressure inlet config? It seems that this is due to this negative pressure peak right in front of the nozzle.

thanks a lot for your help.

Cheers, João

boundary.jpg

[ni-openfoam-user]

I guess at the moment my only comment would be to play with the usual variables (i.e. relaxation factors, time-step)

Also, are you fully implementing your final release velocity? I've found it can be better to ramp up from a low to high velocity over time. In some of our cases for example we also put a H2 cap over the orifice, without these we sometimes get a crash, especially when considering high velocities (boundary going immediately from quiescent air to high velocity h2).

I must admit that this is my first simulation running OpenFOAM, I intend to run a RANS sim and then an LES sim, you seem to have already surpassed me as I'm still having issues with my "open atmosphere" boundary conditions.

I believe I'm going to have to strip my simulation back and then slowly build up the complexity in order to find where exactly I'm having the problem. I guess I was foolish to jump directly from FLUENT to OpenFOAM and attempt to immediately run the final version of the simulation.

Sorry if I'm not much help

[joaofl]

Hello James.

I found that the crash was probably due to the high flow speeds (above mach) on the nozzle's outlet. By decreasing the inlet flow's speed, it stopped crashing. I also found some meshes that I generated, to have to few cells in the nozzle outlet, that was also crashing the simulation.

I'm quit sure of my lack of theory, both from FD and CFD, but sometimes I find more easy to learn if I take an example, and study the effect of the different parameters on it, in parallel with some theory, what gives me intuition, what use to be VERY important.

Like I said, I started from an LES example (pitzDaily), and from that I am trying to grow my solution.

But I'm sure that my next step is to try to find boundaries that do not reflect this waves, since lots of background noise keeps bouncing around.

If you hit the answer and solutions, please share it.

Thanks again!

João

[tomf]

Hi,

For non-reflective boundary conditions I believe there is a boundary condition called waveTransmissive (for pressure), and use it with advective (for other quantities), this may help to reduce the reflections. Both LES and high Mach flow will cause sharp gradients near the outlet (shocks and/or vortices) which means it is likely to have some numerical (accuracy & stability related) issues.

This is not the most trivial to solve. I think there are quite some threads that deal with these issues, I suggest that you look for them.

Regards,
Tom

[ni-openfoam-user]

Hi Tom,

Thank you for answering my request.
Referring back to my simulation (as outlined in the 4th post of this thread, pic of domain attached below, domain dimensions = L x W x H = 18 x 7 x 5.33 metres)

Following your advice I have implemented the following boundary conditions:

For the end (outflow) and top boundary:

• p = waveTransmissive, gamma = 1.4, fieldInf = 101325, lInf = 100.0, value = uniform 101325
• U = advective, phi = phi, fieldInf = (1.1 0 0), lInf = 100.0

For the left and right boundary (longer sides of the 3D domain)

• p = zerogradient
• U = freestream, phi = phi, freestream = uniform (1.1 0 0), value = uniform (1.1 0 0)

I have at the moment switched off the "H2 inflow" so basically I am attempting to run it as an outdoor wind tunnel with 1.1 m/s of air coming in through the air inflow boundary. This is essentially how I want these boundaries to act (open and non-reflecting).

The behaviour has greatly improved, however I am getting a slight increase in velocity from 1.1 m/s to around 1.16 m/s. I would have expected velocity to remain at the initial setting of 1.1 m/s (why should it increase?). The growth of velocity always starts in the bottom right hand corner, at the location of the 'ground' boundary meeting the 'End' boundary.

I have noticed the following behaviour after 3 seconds of simulation time (changing only lInf):

• lInf = 0.5, velocity increases to 2.47 m/s
• lInf = 10, velocity increases to 1.23 m/s
• lInf = 100, velocity increases to 1.16 m/s

I found the following thread quite useful in explaining lInf

http://www.cfd-online.com/Forums/ope...issive-bc.html

(From the tutorials lInf is varied from 0.025 - 5.0)

1) Could you please comment on these results and behaviour, and advise me on my next move?
I plan to now use these settings and start to introduce H2 through the pipe, I have written a boundary condition to start with a low velocity and then increase it over time for stability.

2) From your previous post:
"For non-reflective boundary conditions I believe there is a boundary condition called waveTransmissive (for pressure), and use it with advective (for other quantities)"
What other quantities (if any) should I also be setting to 'advective'
In my 0/folder I have alphat, mut, k, epsilon, H2, O2, N2, p, T and U

Sorry for the long post, but I think its always better to include as much detail as possible.

Kind regards,

James

[tomf]

Hi James,

Did not have time to answer until now unfortunately. Maybe you have already done a lot more research by now.

1) It has been a while since I used the waveTransmissive boundary condition. In that case I assumed an lInf that was approximately similar to the domain itsels and the results seemed reasonable. Also they where not sensitive to the small changes I made in lInf to test. Your changes where a lot larger. Since you have a free jet, it would make sence if lInf is large, also your relative error is smallest then.

2) H2, O2, N2, T and U, basically the variables that are to be advected over the boundary. zeroGradient may work as well.

Good luck,
Tom

[ni-openfoam-user]

Dear Tom,

Thank you again for your response. I am currently running some tests using these settings.

Can I make a further request for some advice?

Using these boundary condition settings at the outer edges of my domain, as discussed, I now seem to be getting the required behaviour, in terms of setting up what it essentially an external wind tunnel. Wind blowing in horizontally from the left and out again through the right. This seems to be fine.

Now I wish to release H2 through the pipe.

Test case details:

Previously I ran a test test of a vertical H2 release through a pipe in the closed box (3x3x3 m) (as you can imagine this was much simplier to set up). the diameter of the pipe was the same (although square pipe rather than circular) and release velocity was 150 m/s.
After say 0.2 s I got a nicely formed jet (please see attachment)

Using the same settings in terms of boundary conditions at the pipe opening and identical settings in the 'fvSolution' and 'fvSchemes' file I then ran this for my open air horizontal release case. As you can see from the attachment the jet is very different after around 0.2 s. Not nearly as well formed.

Questions

1. In your experience is it fair to say that the boundary conditions (waveTransmissive, advective) which were set at the extremities of the domain should have no influence on what is happening at the pipe?

2. Is this more likely to be an issue stemming from convergence settings and differences between the meshes? The release inside the enclosure is much more refined (again please see attachments)

At the moment I am at a loss to understand why these two jets, after the same amount of release time are so vastly different.

• Same release velocity
• Same diameter
• Same solver (ReactingFoam)
• Same version of OpenFOAM (2.20)
• Same settings in 'constant' and 'system' folders

Please recall that I must use this mesh for the Openair release case as I am tasked with comparing these OpenFOAM results to results obtained from FLUENT using the same mesh

Many thanks,

James

[tomf]

Hi James,

1) No it should not, since it seems like the extremities of the domain are far enough away from your region of interest.

2) I would believe the mesh is mainly responsible. As you see in the more refined case quite a lot is happening in the first few cells above the opening. You are trying to capture this all in one cell. So I would suggest to increase the resolution here. Did you get reasonable results with Fluent for this mesh?

Regards,
Tom

[ni-openfoam-user]

Yes, using this mesh with fluent we got quite reasonable results.

(Please see my post above dated August 21, 2014, 16:53)

The top contour plot is the RANS simulation that I am trying to replicate using OpenFoam. I am really only concerned with H2 vol. % at the locations indicated on the plot and not really too concerned with the shape of the jet itself.

I stopped my simulation and increased the nOuterCorrectors, nCorrectors and nNonOrthogonalCorrectors and also added residuals controls and relaxationFactors to see what influence they have have to the solution. It is now running from 0.22 seconds

1. In your opinion is OpenFOAM is more dependent on the grid than FLUENT?

2. Do you have any other suggestions as to what may be going on?

I have an LES grid (as you can see from the bottom contour plot) maybe I should run this RAS sim on this grid to compare if the difference is indeed caused solely by the mesh?

[tomf]

1) I have no experience with Fluent, so I can not comment on this.

2) Convergence within the time step may be another factor indeed, so good that you modified those parameters.

It may indeed be interesting to run at the more refined mesh to see if the jet will develop.

Regards,
Tom

[shenzhou1987]

Hi James!
Recently I'm simulating the jet flow of a nozzle into the air which is similar to your case. As the problem you met before, I don't konw how to set boundary conditions suitably. To be honest, I have used Fluent for a long time, and I'm totally a new one to OpenFOAM. So can you email your case to me? Then I can learn how to do case using OpenFOAM. Hope for your reply.
Thank you very much!

[ni-openfoam-user]

Hi,

I can now help you with your boundary condition settings if you still require?

Kind regards,

James

[aghsin]

Originally Posted by ni-openfoam-user

Hi,

I can now help you with your boundary condition settings if you still require?

Kind regards,

James

Would you please let us know the final situation of your simulation? Would you please share your experience with boundary condition? Thank you in advance.

[virothi]

Hi Tom, which solver would you recommend for the case mentioned above, even I have the same problem and I'm need of suggestions.
Thanks in advance

Originally Posted by tomf

Hi,

For the "Open Atmosphere" boundaries I would use:

p: totalPressure
U: pressureInletOutletVelocity
k/H2/O2/epsilon/T: inletOutlet
mut/alphat/N2: calculated

Regards,
Tom

[tomf]

Hi

any of:

reactingFoam
rhoReactingFoam
rhoReactingBuoyantFoam

The latter if buoyancy is important in your case.

Regards,
Tom

[virothi]

Hi Tom,
I've seen you posting some information which is similar to my need, Could you please suggest which solver I have to use to simulate this gaseous jet propagation in ambient atmosphere.

The jet is pressed through a cylindrical nozzle of a length of 70 mm and an
inner diameter of 1 mm. Afterward, it expands in initially quiescent air of atmospheric pressure. The jet consists of a Helium/Nitrogen mixture of a density of 0.31 kg/m3. The velocity at the nozzle outlet is approximately 200 m/s. Both the air and the jet are of a temperature of T = 293 K. How do I calculate the velocity and mass fraction fields.
Thanks in advance

Originally Posted by tomf

Dear James,

Let me answer you:

1. The reason I suggested "calculated" is due to the fact that the mass fraction of all species should not be larger than 1, using calculated makes N2=1-(O2+H2), assuming your inert species is N2. If you are prescribing it to be only air, you could also use inletOutlet, both should work, I just prefer calculated.

2. Well I have performed similar simulations in the sense that I have had multi-species simulations and simulations with an open atmosphere, but not combined in one simulation. I did however have a multi-species simulation where my outlet was close to a sharp edge, so I used "open atmosphere" boundary conditions for this outlet in order to be able to cope with backflow. The simulation ran fine.

Regards,
Tom

[Y250_MATE]

Hello,

I am having some issues with a simulation i am trying to conduct similar to the ones expressed in this trend. I am basically tring to simulate a jet from an aircraft engine at 600 m/s, 400°K which discharges into a free stream field at 300 m/s (aircraft speed). I am using a rhocentralfoam solver and i am having some weird results that i am not sure it is right. Basically i am having a pressure wave that travels faster than the jet and it bounces back at the outlet of my domain. Once the first wave is damped at the inlet then the flow gets stable. But i am not sure if it is what one should expect.
Can someone offer any help?

Cheers
Raul