We have severe problems in solving an incompressible flow in a straight pipe with swirl. We are trying to solve this assuming axisymmetry (solving a part of the cilinder, piece of pie). We are using CFX 5.5.1 with the default RSM model and air at STP. Whatever we do (local timestepping, transient with smell, 1e-4, timesteps, auto time stepping) the solver always crashes after a number of iterations related to the timestep. The full 3D problem is not a problem. Also using the k-eps model is not a problem (3d or axisymetric). Anybody with some pointers? Did anybody use the RSM model with periodic boundary conditions in any way?

Did you try symmetry plane boundary conditions instead? That might work better. You will have to be careful with your timestep on these as well. i.e., you won't get away with 1/3-1/5 of typical L/V scales. You might need to use 1/100->1/50th instead.

Neale.

It is an axisymetrical tube with a swirling flow (no plane of symmetry thus). We tried it all (timestep wise). Advection time scale is about 1 [s], we went as far as 1e-4 [s]. Still no luck. The full 3D geometry is not a problem. So we are quite sure it is a problem with RSM and periodic boundary conditions. So, no solution yet.

Hi Bart,
Some months ago I tried to solve an axisymmetric problem (a cyclone) using RSM within CFX-4. With k-epsilon everything was ok, but when I started to run with RSM even with first order schemes and very low underelaxation factors there were several problems of convergence. There's a way to reach the convergence for your problem, but it is up to you to find out how to do it.
Another thing, I don't know if it is the way how RSM is implemented in both CFX-4 and CFX-5 in cylindrical coordinates, but when I tried to run the same problem (it was not the same mesh but it really was axisymmetric) with Fluent I've notice no problems of convergence at all.
Regards, cfd guy

CFD guy,

we are not doing it in cylindrical coordinates. CFX 5 does not allow for 2D simulations. We have to do a 3D simulation in a part of the domain with periodic boundary conditions. Apparently it is now an issue within AEA (I hope it still is at least). Aagin the full 3D is not a problem. Until now I haven't got a clue what the problem is.

The problem here is that since CFX-5 is 3D you have to use either periodicity or symmetry to get a 2D axisymmetric solution.

When the Reynolds stress equations are solved you have to make the control volume equations "feel" the rotationally periodic condition. This is easy for the RHS, just rotate one of the flows, add the two flows together, divide by two, then rotate the original flow back. This is trickier for the active coefficients because they become completely coupled under the rotation. The Reynolds stresses are not solved coupled in CFX-5, hence you end up with convergence difficulties when you run with this boundary condition. Maybe the solution for CFX is to solve the Reynolds stress coupled when using rotationally periodic conditions.

I suspect that if you run Fluent or CFX-4 on the same 3D grid, with the same rotationally periodic condition you would have the same problem.

Neale.

Hmmm, looks like a fundamental problem. We are doing some validation cases with turbulence models and swirling flow. When investigating grid dependency we had to loose the 3D tet mesh and go for a more 2D approach. We have a full hex mesh which runs ok but in our day-to-day cases we have to run with a tet mesh. We would like to see whether a tet mesh behaves differently on the validation cases. This is more or less made impossible by these problems

I have also done some test cases of swirling flows using periodic boundaries. With k-epsilon and SST I had no problems with convergence. Similar to your case my calculations crashed using RSM. I didn't find a way through, so I'm off course interested if you find a work-around. Is there anyone reading this thread that has succeeded using RSM on periodic boundaries with/without swirling flows?

Michael Bo

Yes, you are basically right, it is a fundamental problem. Since the Reynolds stress equations are not solved coupled, you can't make an periodic transformation on the active coefficients, only the residual. One other thing you might try is underrelaxing the reynolds stresses. Just add this to your LIBRARY secition in the command file:


VARIABLE: rs
Under Relaxation Factor = real value between 0 and 1
END


The default is no under relaxation. You might have to play around a bit to figure out an optimal value for your particular problem setup.

Neale

I've made a number of simulations using CFX5.5.1 with the Reynolds stress SSG model and with periodic boundaries (rotating flows) - no problems at all.

Besides, why not contact the CFX user support with the problem? - they know their code better than we do and they are paid to solve this kind of problems.

Olav.

Done it. No definitive responds yet. Until now, this (CFD-online) works better. Why have a CFX forum if everybody is requested to take it up with AEA.

Bart,

Just out of curiosity, what are you using for an inlet boundary condition?

Neale

Ah, tricky question. We are doing a validation of an experiment in a vortex tube (part of it). At the inlet we impose the velocity (with outflow in the centre and inflow around that) and reynolds stresses (tried setting them to zero with little effect). So the flow is incompressible in a straight tube with negative axial flow in the centre. CFX5 does it quite good actually with the standard RSM model. The exit is an opening (partly inflow). We are trying the test it with an outlet as well (no results yet)

OK, so are you using an "INLET" boundary condition for your inlet, or "OPENING"??? If you are using an inlet condition, are you seeing wall off? Probably. Did you try just solving the problem without this outflow at the centre of the grid?

Neale

We are using INLET at the inlet. We are currently checking the influence of the exit boundary condition. It turned out to be a very good test case for turbulence modelling AND CFX 5. Untill now we are certainly not unhappy with it

Hi Guys!!

I have had serious problems runnig with RSM in TASCFlow I have observed that a solution for the convergennce in RSM is a very good mesh and a very good initial pre-solutión to begining the run a very small time step and a lot of patience.... Then look the initials values that you are giving for the UU , VV, UV UW,... etc I havew observed in TASCflow that if one start the run with values calculated vased on K (energy) the solution converge if not diverge. But I a not sure about the Y+ on RSM someone of you know how is the best value??

Thank's