I'm having problem running the simulation and non of the guides sovle it ( Layer factor 0.3 and mesh boundarylater blend - disable)
The geometry is cleaned to a level that i'm used to..
simulation is running only when I disable the mesh Enhancement.
Are there any suggestions?
OmkarJ thanks for the reply,
I succeeded to run the simulation with layer factor = 0.05.
Will this influence on the results accuracy?
Just for information, there was no problem to run the simulation in CFD 2013.
Indeed it may, but not necessarily will. Layer factor is basically a thickness of the total prism layers as a fraction of the element on the wall. So having it unreasonably small would mean you will have very small Y+ values and thin prism layer. Now if you use wall functions and your Y+ value is smaller than, 20, you are having incorrect result for wall dominated phenomenon. If you are trying to resolve the boundary layer, then your prism layers would be too thin to cover the whole boundary layer, infusing some numerical diffusion near wall.
That said, it all depends on how sensitive your results are to Y+ values. Separation, reattachment or flows in long pipes where you are interested in accurate DP can be sensitive to Y+ values. But in most cases, the best way is to do a sensitivity study to see the effect of Y+.
OmkarJ, Thanks for the detailed answer.
My case is an electronic enclosure with heat sinks inside - it's hard for me to tell if it influences on the air flow or not..
How can I check the Y+ ?
Well generally, you can't tell if it can, hence I mentioned the sensitivity study. In the same or similar applications where larger layer factors work, you can try running with differnet layer factor and see if your results are too different. If they are, your application is too sensitive to Y+, if not, you should be ok with smaller layer factor.
You can select the variable in "Global" tab as Y+ and view it on the walls. Also, make sure you have enabled the wall Y+ calculation in "Result quantities" in Solve dialogue box. If you haven't already, try running one iteration with that enabled.
I ran the simulation with mesh enhancement 0.05 and got strange thermal and flow results.
I need to manage somehow to run it with the normal value of 0.25~0.3.
In many situations with electronics and the meshing difficulties you are describing, the issue will stem from a small clearance / gap that at appreciable Thickness Factors mesh enhancement cannot fit in to unless it is thinned out appropriately. The best solution would be to find those gaps and to eliminate them (if they are non-critical gaps) or to refine the mesh appropriately such taht ~0.2 (or ~20% of the local mesh size would fit within that gap from both sides).
Easiest method to find these gaps is that once you ahve it meshed, under the design study bar- results - materials - uncheck ALL solid materials such that you only have the fluid visible, then use a Plane and go from one end to the other looking for small sections.