I have slight problems with my model, not that it's diverging but the k and the epsilon doesn't want to converge....here is a screen shot of which values I mean:

H-Energy 2.3E-02 K-TurbKE 2.3E-01 Diss.K 5.4E-01

Any ideas?

0.023 on energy is not that great, and the k-epsilon residuals are less worrying. Is your solution going through some sort of transient stage still? More importantly, what do the u,v,w and p residuals look like, as well as their the global balances? If they are good then you can turn off the u,v,w,p equations using the parameter "solve fluids = f", and ramp up your timestep to some huge value to bring in the other equations in a little faster.

Neale.

Well....the values I posted was just after 30 to 40 iterations. My case is steady state and I've tried to play around with physical timestep and the local one with no results.....any other ideas?

Yes, what do the u,v,w,p residuals and global balances look like? If the residuals are 1e-4 RMS or less, and the normalised balances are less than say 0.1 - 0.5% each then you can probably turn the fluids equations off, and use a larger timestep to bring in energy and the rest. Set "solve fluids = f" while you do this.

30-40 iterations may not be enough to get a converged answer depending on the physics and numerics you are using. For example, if you are running with the high resolution advection scheme or a the specified blend factor advection scheme, it will take longer. 30-40 is possible for upwind solutions.

Neale

Well....first of all...let me describe my model. I got a cylinder that is 15 cm in diameter and 30 cm in length. The flow is axial and the inlet velocity is 63 m/s. Inlet temp. is 26 degrees Celsius and I have a const. heat flux of 3300 all over the body. My simulations so far have converged for a mesh control value of 0.004 and 0.006 (length scale). I use inflated boundary of 10 layers with a geometric progression of 1.2. The ammount of nodes are between 40000 and 80000. I have automatic time step and my residual target is 1E-10 RMS. I've reached that for the mesh control mentioned above but I can't make it converge with 0.002. For the moment over 100 iterations are made and my values for the velocity are at the redion of approx. E-04. For k and epsilon it's E-02 to E-03 and are stable there. Now my question is, if my last mesh is "too fine" or do I need to alter anything in my model to get the convergence I want.

OK, sounds like a simple enough geometry. The fact that you have problems on the finest grid says to me that you might be resolving something that wasn't there before. Have you compared the solution on the fine grid with the coarse grid solutions, maybe you are getting some localised vortex shedding or simliar effect.

I wouldn't worry about the residual levels on k and epsilon just yet. What are your inlet turbulence levels doing? Look at the turblent kinetic energy in for example, does it just die out beyond your inlet, maybe the inlet levels aren't enough for your case on the finest grid. The default intensity is 5% (I think). Does this make sense for you?

If you think that the solution is going transient you can check by setting the expert parameters "backup frequency" and "delete backup files = f". You will get a series of backup files which can be loaded into CFX-Post which might make it easier for you to determeine which area is causing problems. In addition you can also check "output equation residuals" in CFX-Build and see where the residuals are stalling out.

If your finest grid is resolving the boundary layer around the cylinder, then you might also give SST a try instead.

Neale

Well....I solved the problem....the only thing I had to do was to first only calculate fluid eqns and then the rest and this worked like a charm... But now I altered my geometry into the following....I have three cylinders in a row (length of 50 mm and a dimater of 250 mm, i.e. thin ones) where I only model 50 procent of the (using symmetry plane) and the flow is crossaxial. I'm using k-epsilon again and the inlet velocity is 20 m/s and I have an inlet pressure of 20 bar. But it doesn't converge even if I run the eqns separately. Do you think I have to play around with time steps or is it something else that can help me to get convergence. Something worth noticing is that I haven't divergence problems....it just stops converge at around 1E-02 to 1E-03...