Turbulent flow in duct
 

I'm trying to simulate turbulent flow in a straight rectangular duct and calculate the pressure loss. I've created a wall biased mesh and I'm setting up all properties, default k-epsilon model and the relevant boundary conditions. For wall roughness I'm using the same mentioned in the experiment. But pressure loss I'm getting from fluent is much higher than the experimental values.

Can anybody explain what is it that is wrong with my approach or should I change any values so as to match my experimental values??

Thanks.

Did you check the quality of grid? the number of grids(mesh independence test), inflation layer, y+ issue, and so on

Did you consider flow development?

What is the fluid? air or water or else?
If air, did you consider Mach number?

Just guessing here because there isnt really much information, but usually people asking this question ignored that the experimental values were obtained for fully developed flows.
So the first thing you need to check is if the boundary conditions you used in your simulation represent the experimental setup accurately.

Bc's can be accurately matched in this case so won't affect results much (unless input incorrect)..choice of turbulence model and mesh resolution will play an imp. role...use integral model (kw-sst) over wall function ke model. This way you will capture both near wall viscous effects and core turbulence further. If possible use structured o- grid for better control and quality. Grid y+~1 with 10 nodes upto y+~30 will resolve the near wall viscous region and relatively coarser mesh in core is sufficient...hopefully this improve your results...good luck!

Sorry guys for coming back after these many days as I was busy with my course work. I was doing this simulation to study more into turbulence modelling in Fluent. Unfortunately my theoretical knowledge in CFD is very limited as I still have to take a course on that. Mostly I learn from internet.

Coming to the problem, yes I've considered flow development, grid dependence, and I'm using structured O grid, I've calculated the y+ value but I was unable to get the minimum height of cell near the wall to the value I desired as I was unable to get that thickness in Ansys mesh (showing some error! :(). So I generated the mesh with minimum possible height it could generate near the wall. But anyways I'm guessing even if I end up with the required cell height at wall my pressure drop will further increase as this will allow fluent to consider the wall rougness. Is this right?

Also, I've seen some people who would generate a simple tet mesh and calculate the pressure drops in turbulent flows without considering y+ value. Is this correct??
Is there any turbulence model which would consider wall roughness with normal mesh without the need for finer mesh near wall?

Here is the thing with turbulence modeling and wall roughness:

As long as you use a wall-function approach and have y+ values in the range of 30-100 you can model the influence of a wall roughness with some empirical model.

But if you use a wall-resolving approach with y+ values in the order of 1 or below, things chance...
An y+ value of 1 means that the first cell is within the viscous sublayer which extends to about y+=5. But as you learned in fluid mechanics, a wall can be considered hydrodynamically smooth if the roughness height is within the viscous sublayer.
So if there was any influence from a wall roughness, the roughness height would have to be larger than the cell sizes, which basically means that you would have to simulate the roughness directly, using a geometrically rough wall.

regarding the meshing, tet mesh at the wall will be no good, having an inflation layer is compulsory (quoting a cfd expert with 30+ years exp), y+ you can check after the simulation from the contours generated and see if they fall in the desired limit. for the wall losses you will have to give more inputs at the wall boundaries depending on your setup's physics

My guess is that the whole point is in:

"I've created a wall biased mesh "

Could you explain it further? What did you mean with it?

Sorry I just tried to explain it in ansys mesh terms where you use biasing to stack more cells near the edge or at the centre.

Ok, my bad.

K Epsilon is notoriously bad at predicting anisotropic flows in rectangular ducts. Try an explicit algebraic Reynolds stress model.

???could not understand