[abcdefgh]

Hello, I hope you can help me. I currently simulate the pressure drop of a Fluid (Air) flowing through am complex geometry in Ansys cfx. Incompressible fluid, turbulence sst, constant mass flow, room Temperature.
Unfortunately, I get far too little pressure loss compared to measurements (50 % less). Why is this the case?
A Mesh influence study I have done.
If there is no failure in my simulation, how can I increase the pressure loss by simulation? Are there any settings?

Thank you in advance.

[JuPa]

Are your boundary conditions correct - and are they set at the right place?

[abcdefgh]

Thanks for your answer. I think/hope so.
I chose for inlet the velocity. The outlet is a pressure outlet.
What else could cause the wrong solution?

[JuPa]

Is your CFD geometry the same as the geometry for which you have measurements for?

Can you post images?

[abcdefgh]

Yes, its nearly the same geometry. Its a packed bed of spheres in a cylinder. Empircal equations out of puplications are closer to the result from the experiment...so i think the simulation ist not correct.

[diamondx]

have you checked your mesh ?

[Opaque]

Are you meshing the spheres in the packed bed ? If not, it cannot be the same geometry.

I assume the porous media model is being used. In that case, are your settings for porosity, permeability, etc adjusted correctly for your specific geometry.

You have not discussed other details of your model; therefore, we (those in the forum) will be guessing what else may be off in your setup.

[abcdefgh]

yes I'm meshing the spheres. There are the same number of spheres in the same volume like in the experiment. So there is the same porosity. The empirical equations from the literature are only calculated with the porosity...but there is a better agreement between this equations and the experiment.
Only the simulation gets a lower result for the pressure drop.

[fluid23]

It sounds to me like you are probably not using an appropriate turbulence model. If you must know pressure drop very accurately you probably need to do a LES or DNS simulation, not RANS (if that is your current approach). However, that will probably kill you with it's mesh requirements. Maybe switch to k-omega with curvature correction (also called SST) and keep your y+ value as close to 1 as you can.

[fluid23]

As someone else mentioned, you can always model your packed bed as a porous region unless you are specifically interested in the flow around the spheres, not just what comes out the other side.

[jcespada]

have you used the right scaling factor?

What about the properties of the air? are you setting the temperature right? are there temperature changes in the fluid?
the pressure drop goes (quasi) linear with the density...

[abcdefgh]

Thanks for your answers.

I used the SST Turbulence Model.

I think I cantt do a LES or DNS because I have so much nodes and elements in my mesh. An other Turbulence model I tryed - there was no difference.

But could it really be because of the use of RANS?

An other question: how can I use a LES or DNS in Ansys CFX? In Fluent I know it...but ich can't find where I have to set it in CFX.
When I model it as pourous domain, ich have to calculate the Permeability and the pressure drop coefficient...in comparision with the Ergun Equation...is that right? But then it's again dependent of an empirical equation, thats not what I want.

No, I didnt use the scaling Factor. Only in ICEM Meshing, but there is the right dimension.

For the properties of the Air I created a new material with material datas for different temperatures.
But I used dry air datas...in reality I have a relative humidity of 24 %.

At the moment I think its beacause of the mesh...I can't create really good mesh qualities...and its not possible to make prismen layers because of the spheres (they are connected between the middle with small cylinder).
I checked the mesh, there it was ok...but have you an answer how I can do a better mesh?
I did it with ICEM. All Tetraeder. Curvatur/Proximity Based Refinement enabled. With smaller nodes defined by part mesh setup at the wall of the spheres and cylinders.Then after meshing, smoothing to 0.7. Then checking mesh.
I meshed the spheres and the fluid in different icem files and put them together in the setup.

[ghorrocks]

You will need an advanced turbulence license, or a full solver license to have the LES options available. If you only have a simple solver license you will not have these options available.

There is no model option for DNS. You use a laminar flow model, but carefully craft your mesh and other simulation parameters so that it resolves all turbulence scales.

Yes, it is possible a RANS turbulence model may not be adequate to accurately model this flow. But before you give up on RANS you better check if that is likely to be the case. What is the Reynolds number of a typical flow channel? Can you post an image of a typical flow channel? Also post an image of your mesh.

[abcdefgh]

Ok thank you for your Information. I have the Ansys Academic Research License...ist that a full server license? But I've really never seen a LES.

Oh I tried the DNS with Laminar Flow already to show the eddys. Simulation time only 1 s. The calculation is still running.

The particle Reynoldsnummer for packed beds in this Simulation is 6000.
In literature its said, that turbulent flow in packed beds ist from a Re number of 200-300.

[ghorrocks]

Unless you have worked out your Kolomogorov length scales and meshed accordingly, then checked the dissipation is under control then you are not doing DNS.

Re=200 or 300 sounds laminar. Does that mean the flow in the pipe is turbulent but it laminarises in the bed and then can go turbulent again as it leaves the bed?

[abcdefgh]

What do you mean with "dissipation is under control?" When is it under control?
No, in this case I have a Re Number of 6000 in the Packed bed.
But in literature is said, that already at a Re-number of 300 its turbulent, because of the pebbles. But in this simulation I have Re=6000 in the bed. In the bed, there its absolutly turbulent (is said...I hope thats right).

[monkey1]

Using the SAS SST Model wich is available for academic licensing does at least "some" LES
Its a hybrid model that switsches automatically between SST and LES. When LES is possible (mesh fine enough, time step small enough etc...) it does LES and when you have regions where LES does not work it solves SST.

But for your problem I have a totally different guess from all what was said before:
Are you using smooth walls or are you taking into account the wall roughness of your bed?
And why are you using incompressible air?

[abcdefgh]

Thank you, thats a good hint. I'll try that. What will I have to note for the mesh quality? What y+ should be there when I use the SAS SST?

I'm using rough walls (6,3mikrometer) for the pebbles and the wall (only a estemated value)...but I also tried other roughnesses - there was no influence for the result.

And I'm using incompressible air because the Ma number is very small (6,4*10^(-3))...what would be the effekt of incompressible air at this small velocity?

[monkey1]

Hmm got no special advices for the mesh quality. Just try a run, have a look if the model does use the LES and if not hten you should refine (or choose smaller Timesteps). In Post you can easily look it up by visualising the DES Blending Function. Value of 0 = LES and Value of 1=RANS.

You know that the wall roughness to fill in in CFX is not equivalent to the "real" roughness? There is a chapter somewhere in the documentation where they describe that (if I remeber correctly) the CFX Roughness is approx. 30*real roughness.
But in my simulations I also never noticed a relevant influence (but I'm doing atmospheric dispersion, so that the roughnes is only secondary).

Oh ok with that low velocities I don't think the compressible fluid would make a change. I was thinking you had higher Velocities. Your figures showed velocities around 30 m/s which would give a Mach number of around 0,1 no? It would still be in the "incompressible" region below Ma=0,3 but at 30 m/s and small orifices I would at least have tested if it makes a difference.

[ghorrocks]

What do you mean with "dissipation is under control?" When is it under control?

Dissipation is a critical factor to consider in DNS simulations. If you intend doing the DNS approach you must get some turbulence modelling textbooks and understand this factor.

If you are not doing DNS then don't worry about it. I suspect that it will not help you so I recommend you use LES or RANS. Monkey's suggestion of SAS sounds good to me.