[rap7or]

Hello everybody, I have a weird problem. I am simulating a combustion process with a de laval nozzle. Into the exhaust plume, particles are injected. They accelerate, melt and impact on a substrate to build a very hard layer against corossion and wear. I am simulating this process in 2D axisymmetric and 3D. With the same settings I get completely different results. The problem is I have to simulate 3D to be able to recognize, how the particles are moving in the stream (I use DPM stochastic tracking for this and it works perfectly).

Here is the 2D axisymmetric result:




And here the 3D result:



What the 3D problem is, is that the velocity and the temperature of the fluid decrease far to fast. In the 2D axisymmetric solution, the plume is realistisc in terms of diameter, velocity contour etc.

My settings are

* Transition SST
* Species Transport with volumetric, eddy-dissipation reaction (n-Octane-Air)
* DPM with stochastic tracking (for the fuel droplets and particles for coating)
* mass-flow-inlet (Species: Only O2)
* Pressure-Based Solver
* Ideal Gas model for the species transport
* Viscosity: All on sutherland
* Transient: 1e-5s per timestep
* Pressure: Presto!
* First Order Upwind Transient Formulation

[RaiderDoctor]

The only thing that I can see so far is that the 2D and 3D geometries do not look to be similar. For instance, on the 2D model, the enlarged structure on the right has angled lines, whereas on the 3D model it looks like they are flat. Also, the narrowed section looks different for both models somehow.

This may be a very dumb question, but are your geometries the same?

[rap7or]

Originally Posted by RaiderDoctor

The only thing that I can see so far is that the 2D and 3D geometries do not look to be similar. For instance, on the 2D model, the enlarged structure on the right has angled lines, whereas on the 3D model it looks like they are flat. Also, the narrowed section looks different for both models somehow.

This may be a very dumb question, but are your geometries the same?

yes they are. it s just that my fluid exhaust room is bigger so i moved the 3d room a bit to the right for optical comparison. chamber pressure an d temperature are exactly the same. only the exhaust plume decreases far to fast in 3d

[RaiderDoctor]

I mean, I'm still not convinced that they aren't different geometries. On the 3D, it looks like the exhaust is way bigger than that on the 2D. The exhaust on the 2D looks to have the same diameter as the inlet area, but on the 3D it's a lot bigger.



Also, I have to ask if these are taken at the same time step. Not only does the plume in the 3D look different, but the inlets look exceedingly different as well.

[diggee]

Originally Posted by rap7or

I am simulating this process in 2D axisymmetric and 3D. With the same settings I get completely different results.

The 2 geometries are not the same. The 2D axisymmetric geometry has gradual expansion whereas the 3D geometry has sudden expansion. The sudden expansion will make the fluid behave like a jet and what you have got is what is expected, at least within the visual limits. Further, the gradual expansion affects the fluid mechanics in the expansion region; the recirculation bubble in sudden expansion is bigger than that for gradual expansion which will then affect the plume size. IIRC, there is even a bare minimum expansion angle that has to be satisfied for a recirculation region to exist; somewhere around 9 degrees or so. I am sure that if you made the 3D geometry just like the 2D one, you will get a better match.

[RaiderDoctor]

Originally Posted by diggee

The 2 geometries are not the same. The 2D axisymmetric geometry has gradual expansion whereas the 3D geometry has sudden expansion. The sudden expansion will make the fluid behave like a jet and what you have got is what is expected, at least within the visual limits. Further, the gradual expansion affects the fluid mechanics in the expansion region; the recirculation bubble in sudden expansion is bigger than that for gradual expansion which will then affect the plume size. IIRC, there is even a bare minimum expansion angle that has to be satisfied for a recirculation region to exist; somewhere around 9 degrees or so. I am sure that if you made the 3D geometry just like the 2D one, you will get a better match.

Thanks for seeing what I was seeing, haha. Also, I starting thinking about something else as well; how different are your meshes? Could you post a snapshot of your 2D mesh, and a cross-sectional area of your 3D mesh for comparison?

[rap7or]

I ll defininetly try your recommendations out and will give complete feedback later this evening. Thank you very much for your advice. I ll make the geometries completely similar with exactly the same boundaries and mesh etc. plus the angle you said in terms of recirculation.

[RaiderDoctor]

Just checking in to see how your problem is going.

[rap7or]

Well I kind of improved the situation, but still struggling with the 3D Model itself. I got it up running in 3D with two symmetry regions. But when make the model 3D without symmetry, the whole combustion process doesnt work anymore. It does some weird stuff by not reaching the normal combustion temperature of about 3,500 K.

I have exactly the same settings in the 3D model without symmetry. In the attachments you can see the results of the 3D with 2 symmetry regions.

I am basically struggling to create the long exhaust plume and reaching the right combustion temperature and pressure in the complete 3D model.

[RaiderDoctor]

I think there might be some typos in your previous answer:

We were previously working with a 2D axisymmetric geometry and a 3D geometry. Now, it seems like you are running a strictly 3D geometry that can either be, 1) purely 3D and 2) a quarter of the entire model with two regions of symmetry.

The first question I have to ask is what do your meshes look like? Are they exactly the same? And by that I mean does you symmetry-model mesh have a large number of cells on the symmetry faces that would increase the solution accuracy in this region, whereas you 3D model just has a uniform element distribution?

Second question would be how long are you simulating these cases for? You mentioned a time step size of 1e-5 s, but what is the end time? Finally, can you post a picture of both cases so that we have a better understanding of what is going on?

[rap7or]

after 6 weeks i finally found the answer to this problem. i got the density-based solver running, just without the combustion, and modeling the chamber pressure as an pressure-inlet. the results from the exhaust plume were very close to the measurements in reality.

now i just have one problem with the combustion. do you guys recommend specific options for the density-based solver combustion? like i get far too low chamber pressure and the eddy-dissipation model does not work very well (it worked perfectly with the pressure based solver and the chamber pressure was 5% away from reality).

my settings are:

*eddy-dissipation
*droplet injection (surface, kerosene-droplet, 50 µm size, etc.)
*at the droplet inlet i have a velocity-inlet with 100% oxygen