Mesh size and solver residuals...
I have a simple pipe flow problem, where the flow makes a 90 deg change in direction at the intersection of two pipes. There is no radius/bend at the intersection, so there is some flow separation and recirculation at the corner. The fluid is water, Re > 20,000.
The pipes I'm modeling have an ID of about .25". The mesh element size throughout most of the pipe is on the order of .050". In the area of pipe intersection, I have refined the mesh element size to be on the order of .025". I have 15 layers of inflation, with approximately 10 of those layers within the estimated hydrodynamic boundary layer thickness. When I attempt to solve this simulation in steadystate, with an SST turbulence model (5% inlet turbulence) and all initial conditions set to auto, the momentum and turbulence residuals approach 1e4 after about 40 iterations, but then start to fluctuate and slowly rise, never reaching convergence. When I attempt to solve this simulation using the ke turbulence model, I reach a 1e4 residuals convergence on fluid momentum components after 120+ iterations, but just barely. For the ke model, if I plot the abs of the momentum residuals, the cells that still have high (>1e4) residuals are those where the flow is experiencing separation and/or recirculation. See the following photo (u momentum residuals plotted with gray volumes): http://74.220.219.65/~scottpol/image...wResiduals.jpg I have tried further mesh refinement in these areas (decreasing the element size from ~.025" down to ~.01"), but it actually made convergence worse. Does anybody have any suggestions on modifications to my mesh or model setup that might help me reach a definite and accurate solution without oversimplifying the flow? I appreciate the help. Thanks! 
Re: Mesh size and solver residuals...
Hi Scott,
The high residuals indicate the flow is changing significantly in these cells. In your case the change is due to velocity fluctuations at the interface; similar to turbulent vortex shedding, though the steady state solver will not be resolving these directly. Refining the mesh will make it worse because your are increasing the velocity gradient (by getting closer to the shear layer) and also allowing the mesh to transport smaller turbulent" features. Try increasing your timestep. Since CFX uses a false timestep, increasing the timestep will allow the solution to propegate further at each iteration. This may wash out the fluctuations and help converge the solution. CycLone 
Re: Mesh size and solver residuals...
Thanks for the reply. I've played around with the timescale a little, but perhaps not sufficiently?...
The advection time for my model is about .2 sec. I've tried setting the physical timescale to .2 sec, 2 sec, and 20 sec, but the convergence using ke turbulence doesn't seem to improve much (if anything, the convergence appears "bouncy" at the higher timescales), and I wasn't able to achieve convergence using sst turbulence at any of those timescales. Any thoughts on setting the Gradient Relaxation or Blend Factor Relaxation? I'm not familiar with these, but I see some references to them in the "Problems with Convergence" section of the help manual. Thanks again, Scott 
Also...
I forgot to mention, I have been using double precision to solve this model.

Solved...
Here's how... I ran the model to a 1e4 rms convergence with a ke turbulence model and the fluid timescale set to 10x my advection time (case 1). Then, I ran the model again to a 2e5 rms convergence with a timescale of 1x my advection time, using case 1 results as the initial conditions (case 2). Now I'm running it a third time with a timescale of 0.1x my advection time, to rms residuals of 1e5, and it seems to be on the path towards convergence. Sweet.

Re: Solved...
Good to hear you are on the path to convergence. You might find this a useful reference in future:
http://www.cfdonline.com/Wiki/Ansys...gence_criteria 
All times are GMT 4. The time now is 05:06. 