I was trying to model pressure loss in a complex duct and getting results that made no sense.
So ... I went to the simplest thing I could think of 12" of 4" diameter duct with constant flow of 350 cfm.
tried automatic, manual, adaptive, enhanced meshes of various densities and geometries.
No matter what I did, I could not get close to the known loss of 0.0707 inches of water.
often (VelocityPressureOut - VelocityPressureIn) was the wrong sign !!
boundary conditions: input 350 cfm, output 0 psig
initial conditions: everything at 68 degrees
what am I missing ?
Solved! Go to Solution.
I would stick with the original ducting and troubleshoot that, with the correct inlet and outlet lengths we can hit the figures for a straight pipe.
Would you like to share your original model and what you are expecting vs what you are seeing?
I would add (a rather obvious point) that it may be helpful to use extensions before and after your ducting so the BCs do not influnence the domain too much. Correct interpretation of static pressure drop can be obtained only after the pressure recovery has taken place after any fow disruption in ducting. Taking pressure drops too close to the disruptions may result in wrong sign, because pressure has not yet recovered.
ok, went back to the original design (I extended the inlet and outlet) and ran the cfd analysis again.
it's still wacko.
the numbers from the Decision Center say the pressure drop is 0.835 inches of water column
the correct (measured) result is 5.27 inches of water column.
I am at a loss ...
This is a cyclone model, just for anyone else's reference.
Actually pretty tough to model and very mesh sensitive. The turbulence model you chose should get us as close as we can.
- Extend the inlet and outet but about 2-3x
- Suppress all solid parts from the mesh - saves on memory
- Refine the mesh - to about 0.2 is a good start
- Tighten the convergence assessment or simply turn it off - it will take a while for the cyclone to develop
That should give you a decent start. I am going to ask a colleage to check on this also as I know he will have some advice.
You can get reasonablly looking flow results in a cyclone, but the pressure drop is going to be off. This type of model requires a turbulane model that Simulation CFD does not have.
Before I saw the message from Royce, I tried Jon's suggestions, plus using a non-zero
surface roughness coefficient for the walls ... not much difference.
The lack of the proper turbulence model certainly explains the wacky pressure results.
Are there plans to implement something like the large eddy simulation (LES) or the
Reynolds stress turbulence model (RSM) found in something like FLUENT ?
Do you think the existing 2-eqn models are not suitable becauase strong curvatures to streamlines and strong secondary flows will render the assumption of isotropic turbulence in 2-eqn models unsufficient? While RSM or non linear k-eps models can be an alternative here, how about using the new SAS model? Sufficiently fine mesh at the core region of cyclone and smaller timestep will mean that area can be captured using LES? The computational expense will be mammoth though.
I did try both the k-epsilon and SST k-omega SAS turbulence models
As suggested in the notes, I did use enhanced meshing with 10 layers
I did use a mesh adjustment on the air volume of 0.2
I did use10 iterations of adaptive mesing
There were several million fluid elements in the last iteration, concentrated along the surfaces.
But then again I did use the same setup on a straight 10' section of 4" duct and had similar
difficulties in getting a value for pressure loss which agreed with measurements.
I do respect the difficulty of the problem, yet CFD programs do generate useful results.
The notes say that pressure loss through a duct was validated ... perhaps you could send me this
setup, so I could learn what your program needs to get results which agree with measurements.
SAS is a combination of LES and SST-kw but it is tricky. If you don't have adequately fine mesh, it just solves using standard kw-SST instead of LES. It is believed that you need a mesh size of the order of Taylor's lengthscale and timestep really small so that you are able to resolve the eddies in inertial subrange. In other words, you really need to be knowing what you are doing here, otherwise you don't have LES results. Moreover even if you use really fine mesh in the zone of interests, it still is unstructured tet mesh while in LES, generally a structured mesh is recommended. At the same time, you don't have a liberty of using the recommended central difference advection schemes for LES. So there are some caveats with SAS which may affect your solution. Royce may comment on the conjecture.
How about posting the idea for RSM in Idea Station? Will vote it up!