Hi I am trying to model a S-Duct with high mass flow at the outlet but the results do not match with the experimental data. The outlet is semi-circular 6 inches diameter and the inlet 7 inches. Mass flow rate at the outlet 1.48 kg/sec.

Please tell me if there is anything i can do about it. I am using CFX-5 and ICEM Hexa (500000 hexa element geometry)

Hi Fotis,

Getting accurate answers with CFD requires skill, experience and lots of patience. Read the literature and see how other people have done on similar problems. Obvious things to look for problems include:

• <LI>Mesh density - have you reached grid independance?</LI> <LI>Turbulence model - are you using an appropriate turbulence model, with sensible wall conditions?</LI> <LI>Upstream/downstream boundary - are your upstream and downstrream boundary representative of the experimental results?</LI>

That's the first few things to check.

Glenn

Hi Glenn

The generated grid is fine,smoother at the walls and i think it's the best i can make. I am using SST model witch seems to be the most suitable for the problem. Upstream and downstream conditions are representative of the experimental results because i have two test cases for comparison. The first with low mass flow rate gives simmilar results as the experimental ones. The sesond is difficult because of the shockwave that grows near the inlet of the S-DUCT.

Is there anything more that i can do for setting sensible wall conditions;

Hi Fotis,

Why do you say "the generated grid is fine"? The most likely cause of the problem is the grid is not fine enough.

The SST model should be a good turbulence model for what you are trying to do.

You mention a shockwave - that means you are doing fully compressible flow. This is much more challenging than incompressible flow. You are likely to need a really fine mesh around the shock to get accurate resolution. Mesh adaptation is good for this type of simulation.

Glenn

Except that they are running a hex grid in CFX-5, in which case mesh adaptation sucks because it makes some elements into pyramids, refines boundary layers, etc... due to no hanging nodes being supported. This kind of refinement might kill a boundary layer flow.

Fotin, you need to closely look at the flow and figure out what physical behaviour is causing the non-matching to experimental data. If you are getting a converged answer then the flow solver will basically do something physical based on the boundary conditions you have specified.

Maybe the shock is in the wrong spot so it trips the boundary layer too early, maybe your exit boundary condition needs to be further away if the shock is hitting it, etc... there could be many reasons, you need to use your judgment.

If you even have a shock that means the flow is going supersonic somewhere, so perhaps a mass flow exit condition is really the wrong thing then becuase this is really a subsonic boundary condition. Maybe you need to take a closer look at why the flow is "shocking" at all. Is it supposed to?

So many reasons for getting an unexpected answer.... Generally it is not a problem with the flow solver.

Neale

Hi,

Good point Neale. The structured mesh means automatic mesh refinement will not work well. Automatic mesh refinement can be very useful in resolving shocks accurately, so it might be good to switch to a tet/prism mesh so automatic mesh refinement works.

Glenn

Is this the same S-Duct as on the NPARC website?

Neale

Hi Neale & Glenn

Yes its the same. The experiments are also present on Agard report AR-270, named Test Case 3.1 & 3.2 . The outlet is far away the area that shock exists I would try to make a simulation with Tetras and prism mesh adaption and compare the results.

Thanks anyway

[ADNAN PMI]

can u plz attach some photos of ur mesh file and what are the boundary conditions u've gievn.?